Our CNC software is designed expressly for the Plasma and Oxyfuel Flame Cutting Industry to exploit the many technological advantages only available from our intelligent motors. New users and seasoned users alike will appreciate the ease of operation provided by this software.

Our CNC software can accept traditional G-code or drawings in a DXF file format. Objects created in many of different software packages are easily imported using DXF file formats.

The DXF Conversion screen of our software allows standard DXF files created by any CAD or drawing software to be imported, and converted into G-Code that is used to direct cutting operations. Additionally, the DXF files can be processed to optimize them for plasma and oxyfuel flame cutting.

The following two sections will help you get started.

CNC Plasma Cutting 101

A tutorial on Plasma Cutting

Quick Setup

A quick guide to get your plasma table set-up to the correct operating parameters

CNC Plasma Cutting 101

CNC plasma cutting, like many other disciplines, has unique attributes and methods. We hope to give a new user some basics as an introduction to this fascinating and useful subject.

A plasma cutting machine typically takes ordinary compressed shop air, strips off its electrons converting it to a super hot ionized state (plasma). A hand held or machine operated torch projects the super hot plasma against the material to be cut. When the plasma hits the material it melts; the melted material is blown away by the force of the moving plasma leaving a hole or gap. By moving the torch across the material, a continuous gap is created much like one created by a saw blade. A hand held torch is limited in accuracy by the hand that holds it. A machine torch is a specialized torch designed to be held and moved by a computer controlled gantry system, which assures accuracy in complex cutting operations.

There are two types of CNC plasma cutting systems: Standard and High Definition. High Definition systems utilize the same ionized gas principle but different torch design and gas feeds. High Definition can produce cleaner, more precise cuts than standard plasma cutting systems but generally cost as much as $30,000. For the purpose of this discussion, we will stick to Standard plasma cutting at a small fraction of High Definition costs.

What can you do with a CNC Plasma Cutting Machine? Essentially, you can cut simple or complex shapes into any material that can conduct electricity. Typical materials would be common steels and aluminum. Non-typical materials might include brass or copper titanium (creates toxic fumes) with special provision for venting, vision protection and gas selection. Complex shapes can be cut into flat stock, tubing, angles etc. Cutting can be done rapidly, accurately and with repetition. Cutting parts for mechanical assemblies or artwork of great complexity can be accomplished with equal speed and accuracy.

Can you cut watch gears with a CNC plasma cutter? No, and you can’t engrave on diamonds either. The gas-like plasma removes material while it cuts much like a saw blade cutting a board. Like any device that removes material while cutting, plasma cutters have limitations on doing very small detailed work. However, small work without tiny inside radiuses is well within its capabilities. Additionally, formerly tedious tasks like locating a pattern of holes can be done through a series of pierces for later drilling to finished size. This can save many hours of layout work. We have cut a number of ¾” by ¾” parts with a located hole in the center many times. Because of its low cost and high versatility, plasma cutting has become a fabrication tool in thousands of shops.

How does an object go from a drawing to finished part? First there is software. CNC plasma cutting requires three basic types of software: creation, conversion/modification and execution.

Creation software actually generates the drawing that will be cut. Parts for fabricated assemblies are created by CAD packages like AutoCAD, Turbo CAD and many others. These CAD systems have a universal export (interchange) format called DXF. Drawings produced in a DXF format can be easily imported into most plasma cutting systems. DXF drawings are in a vector format as opposed to a raster format. Vectors are lines of specific length and direction. Raster formatted drawings are made up of a series of dots. Bitmaps and “Gif” drawings would be examples of raster images. Although the human eye can interpret raster images, a CNC machine can not. Raster images must be converted to vector format. There are many ways to do this. Some methods are good, some bad. You can call us for a further discussion of this subject. AutoCAD, Turbo CAD, Corel, PhotoShop and dozens of others can provide you assistance in creating drawings suitable for importing into your plasma cutting system. Since excellent drawing creation software is available on the open market, we leave it up to the user to select what is best for their unique needs. If you need some help in that direction? Call us. We are anxious to help.

As mentioned, the plasma cutter removes material while cutting. The width of the cut, as an example, might be .040. If we center the cut on the parts edge, we will remove .020 off the part’s edge. This will produce an undersized part. If we offset the cut .020 into the waste side of the material the part will be properly cut. Specified offsets can be created in most good CAD packages.

At the start of each cut the plasma cutter makes an initial round pierce. From the pierce hole the CNC plasma cutter begins cutting its normal slot. If we were cutting out a box-shaped object and began with a pierce at one corner. The round pierce hole would nip off the corner a bit and leave that corner poorly formed. To prevent this, we pierce the material a short distance away from the object, start the cut and proceed into the object with a fully established, clean cutting arc. The cut from the pierce point to the beginning of the object is called a “lead in” (see figure 1). Similarly we want to terminate the arc away from the object, so we continue the arc a short distance beyond the normal completion point. This is called a: lead out.”

CNC machines move according to very specific instructions given to them. These instructions are in the form of a CNC machine programming language. This programming language is called G and M coding. Since the typical drawing input format is a DXF file we need some way to convert it to G/M code. Some CAD software can save a drawing directly in a G Code format skipping the need to convert a DXF file. As part of its structure our software provides a simple means of converting DXF files into G Code.

In addition to doing a G-Code conversion our software does much more. Typically a DXF drawing file generated by a CAD package needs a bit of “tuning up” to optimize it for CNC cutting. For example, a drawing may need to be joined. Picture a drawing of a box. The box may consist of four separate lines at right angles, or, it may consist of one line with four right angles. This is a big difference. The CNC Plasma cutter will interpret the separate line box as needing four independent cuts and will stop and restart at each corner. This will produce a sloppy part. The CNC cutter will cut the one line box differently. It will start at one corner and cut all around the box without stopping till it returns to where it started, which results in a much better part. Our software allows you to take separate lines, arcs, etc. and join them into one line entity for optimum cutting.

A drawing may need to be sequenced. Imagine you want to cut a donut. If you cut the outside circle first, the part will drop out of the material stock and you will not have the opportunity to cut out the center hole. When a CAD program creates a drawing, the order the drawing parts were created in is the order they will be cut. In most cases the order they were created in will not be the order you want them to be cut. Our software allows you to reorder the cut sequence to your choices.

Once you are satisfied that your drawing is properly joined and sequenced, the software should be able to save it as a G-Code file. When the G-Code is created you have completed all the work needed on the drawing file and it is ready to cut.

The execution portion of the software will then process the G-Code into the drive components and cut your parts.

At this point we should discuss the steps involved in plasma cutting.

In the first step the torch needs to properly locate itself above the material. That the torch must be over the proper location to begin the first cut is obvious. What may not be as obvious is that the torch must also be the proper distance above the work. To do this the torch must locate the material in relation to itself. There are three basic types of material sensors the torch can use to “find” its initial height above the material. The three sensors are: a mechanical switch, proximity and pressure sensing. The torch positions itself over the starting point, lowers itself, finds the material using one of the three sensing methods, then raises itself to an optimal height for an initial material pierce. Do not confuse the pierce height and cutting height. The pierce height is larger than the cutting height. When piercing there is a momentary molten material splash. You want the torch tip high enough to avoid the splash fouling the torch tip, but close enough to make a clean pierce. Once the material is pierced and arc established the torch should lower itself to an optimal cutting height.

Maintaining the proper gap distance between the torch tip and material wile cutting is critical. Anyone stating otherwise is being less than honest with you. Material as received from the mill is not perfectly flat. Material that may be reasonably flat will bow somewhat while it is being cut from heat warpage. If the material to torch tip distance is not maintained within a few thousandths of an inch, regardless of the material’s flatness, the cut will be poor and torch tips will not last. Maintaining the proper distance is the job of an automated torch height controller. Without an automated torch height controller there is NO way to maintain proper cutting (arc) gap. Again, some type of automated torch height controller is essential from day one. The best types maintain cutting gap by monitoring arc voltage. The best types can set an initial pierce height and maintain a separate cutting gap distance. Of course, our torch height controller can do both exceedingly well.

The plasma cutting arc produces an angular cut called a kerf. This means the cut edge may not be perfectly perpendicular. The thicker the material that is cut the more pronounced the kerf angle appears. Kerf angularity can be minimized by keeping in mind this rule of thumb. Using our donut as an example, cut the outside circle in a clockwise direction. Cut the inside circle in a counter clockwise direction.

While a cut is being made some of the oxidized material removed by the plasma arc is not completely blown away. It sticks to the cut edge in droplet form. This material is called dross or slag. Dross is very brittle and is easily removed by tapping it with a small hammer, grinding or sanding it off. The amount of dross produced is a function of cut speed, torch tip condition, material cleanliness and material quality.

Quick Machine Parameters Setup

BE SURE YOUR MONITOR IS SET FOR 1024 BY 768 DISPLAY MODE

This section includes step-by-step instructions for setting up your software and calibrating your machine for the servo drive software.

Hard stop installation for Hard Stop Homing

Hard stops are to be installed at the X and Y travel limits.

These are physical blocks that prevent the machine from moving off the rails and limit travel. If this is a retrofit installation you should supply these to your existing machine. If this is our gantry, the Y-axis will already have stops. The small “C” shaped stop blocks will be supplied with the rails and should be installed at each end of the X-axis rail over the small gear rack and clamped with the screw.

Go to the Setup menu and choose Machine Settings. Here you will find all the Machine parameters. We will go over each tab that is necessary to get the basic machine settings in place for correct operation. When you click on the tab listed, adjust the settings to match your machine:

Machine Settings Tab

Motor Encoder Pulses = 2000 for X Y and Torch (and Slave if applicable)

You will need to adjust the Work area plus limits to match your table size. For a 4'x8' use X=96”and Y=48” for a 5'x10' use X=120” and Y=60”. Set the Torch at 0.0. Later on, after you home the machine and jog the machine to these limits, measure how much more travel is available and add this to the limits.

Work area minus limits to -0.1 for X and Y then set -4.0 for the Torch.

Scaling with our 30 to 1 gear reducer X=-15275, Y=15275, Torch = -10000 (new)

Scaling with our 28 to 1 gear reducer X=-14257, Y=14257, Torch = -10000 (old)

If you have built your own gear drive system, please calculate the number of pulses it takes to move 1"... the motor encoder has 2000 pulses per revolution. Or press the "?" button for help with this calculation.

Maximum Velocity please start with 12 inches per second for X and Y, 15 for Torch

Rapid Accel please start with 10 inches per second for X and Y, 12 for Torch

Cutting Accel please start with 4 inches per second for X and Y

If any RPM indicates greater than 7000 rpm, you are destined to have failures. Please lower the maximum velocity, until you reach about 6000 rpm as a maximum.

On Dual Drive units, never exceed 5000 rpm on the slave motor

Inputs Tab

Go to Setup, choose Machine Settings and then select the Inputs tab. Adjust theses settings:

Port B input on X axis = Plasma Arc Confirmation

Port C input on X axis = Emergency Stop

All other ports = Input does nothing

Homing Tab

Next, select the tab marked Homing and change these settings

X-axis

Opposite is Checked

Y-axis

Opposite is Unchecked

Torch axis

Opposite is Unchecked

All axes

Velocity is 3/4 full

Ignore in Unchecked

Torque = 120

Offset = 0.25

Home Value = 0.0

Tuning Tab

Now select the tab marked Tuning and verify these settings

All Axes

Proportional gain = 30

Derivative gain = 300

Integral gain = 15

Accel Feed forward = 0

Integral limit = 100

Follow error = 7000

Sample rate = 1

Velocity feed forward = 0

Gravity compensation = 0

AMPS = 1000

Additional Parameters = F=8 (no spaces between F=8)

Advanced Settings Tab

Select the tab marked Advanced and verify these settings:

Ask to Home at Start is CHECKED

Show user defined is CHECKED

User Down = 03

User Up = 05

If no feed rate... is CHECKED with a value of 100 ipm

Allow re-zeroing is Unchecked

Keyboard character W turns on 7

Outputs OFF when error = 7

Feed hold outputs is CHECKED with value = 7

Resume outputs is Unchecked with value = 0

Wait for M50 is Unchecked value = 0

Do NOT reset line number is CHECKED

Start Cycle with line number... = 0

M30 turns outputs off = 7

Vertex slowdown = 45 degrees

Continuous path is CHECKED

Slow at Vertex is CHECKED

Allowable overshoot = 0.05

Max comm errors allowed = 1

E-Stop abruptly halt motor is UNCHECKED

Show Subroutines is UNCHECKED

Enable view options is UNCHECKED

File open extensions should include tap, cnc, nc, txt

Under the value for the default feed rate (located left center) you may set a default feed rate if you do not have one in your program. If you use a value of 100, then the feed rate override percent on screen can represent the actual feed rate.

Colors and line widths may be set to any user preferences.

Torch Tab

Next select the tab marked Torch and verify these settings

Scaled Arc Voltage = 5.0

Down force for searching = 80

AVC Height sensing delay = 0.75

Arc output ON delay = 1

AVC Correction sensitivity = 9

AVC # of measurements = 15

Fixed distance jigging Z = 0.0625

While cutting Jog Moves = 0.0625

Number of seconds to wait for arc = 5.0

Delay time after arc established = 0.0

Raise torch between cuts is CHECKED

Using jog buttons... is CHECKED

Pause at pierce height is CHECKED

Output for Cutting Oxygen = 2

Output for Preheat = 4

Leave preheat gas ON is UNCHECKED

Joystick Tab

If you have a joystick connected to your PC and you have calibrated it from the windows control panel... then select the tab marked Joystick and check the enable box.

Using this page as a training aid and key. you can simulate inputs and see what functions are available. See later section for notes on the proper use of the joystick when cutting.

Offsets Tab

Next select the Offsets tab.

There are two user defined position buttons at the bottom of the page. The first is the Torch service position and the second is the Material load position. These are available at all times. Clicking in either of these buttons will raise the torch and send the machine to the specified location immediately. The valid coordinates must be within the plus limits set on the Machine tab of the settings.

CHECK the Raise torch boxes and enter the positions for material load and torch service ONLY leave all others as they are for now.

Now select “APPLY” at the bottom, confirm and then “CLOSE” the machine settings. All of your settings are now ready to operate the machine.

Drive Direction and Homing

*Note: If a drive errors out, the coordinates at the top of the screen will go gray and no movement is permitted. To turn them back on, select the check box button in the far left upper section marked ALL ON to turn them back on. All drives should be on when operating the machine.

1. With the machine power off, push the machine to the middle of the table. This will prevent you from running off one end or damaging anything. Power up the machine and start the software by double clicking on the icon on your desktop. Do not attempt to home the machine yet. When asked to home, click NO!

2. Select the check box on the screen under jog direction for 1/10 speed. Start with slow moves to avoid damage.

3. Jog the machine using the jog buttons on the right side of the screen. The machine should move away from you on the short axis for Y+ and to the right on the long axis for the X+. If not, go to Setup, Machine Settings, Machine tab. Change the sign from + to -, or vice versa for that drive axis scaling; do not change the number yet. Click on “Apply” and “Close” then re-check.

4. When the machine moves in the correct direction, jog towards the limits and stop about three or more inches away from it. Now go to Setup - Search for home and pick the X-axis. If the machine moves away from the limit right away, press escape or click the “E- Stop” button on the right-hand side of the screen. Go to back to Setup, Machine Settings and select the Homing Tab. Invert the selection in the box marked “Opposite” for the homing direction. Click on Apply and then Close Try again. Repeat this process for Y, and if equipped, Z (Torch) axis. The speed of the homing routine is also adjustable on the Homing page. After the machine has homed for that axis, you may want to repeat the process and observe where it stops. This is your zero position. You can make some changes to this by setting the Offset and Home Value. The offset tells the machine to move away from the hard stop by this amount either + or -. Once complete, the Home Value will be applied to the final position.

5.You my now home all axis when starting the program, or at any time by going to Setup, Search for Home, Home all Axis.

Drive Distance calibration and Speed Setting

NOTE: THIS STEP SHOULD ONLY BE REQUIRED ON RETROFIT OR CUSTOM INSTALLATIONS OR WHEN YOU WISH TO CHECK MACHINE ACCURACY CALIBRATION. OUR GANTRIES WILL ALREADY HAVE THE CORRECT NUMBERS (15275) LOADED

1. Home the machine and mark the machine's position with a piece of tape for reference.

2. Go down to box in the lower right next to the arrow. You can enter manual code directions for the machine here. Type in a command to move 10 inches to the X+ direction as: “G0X10” and press enter. (G0) is a rapid move. *Note: (G0) is (G zero) not the letter “o.”

The machine will move to the X+ a distance. Measure this and record. Type in “G0X0” to return to the zero point.

You can also simply choose FIXED in the jogging window, and select value of 10.0. Clicking on the X+ arrow will move the gantry 10", clicking X- will move it back 10"

Calculate an encoder distance as follows:

Commanded move (10) / Actual move (insert distance measurement)= correction factor

3. Go to Setup, Machine Settings, and under that axis, look at the box marked Scaling Multiply this number by your correction factor and enter the new number. The X and Y numbers will usually be the same.

4. Repeat the 10-inch move command and recheck. Repeat any correction still required. When satisfied, repeat this process with a long move to look for error accumulation. You may also use a dial indicator for a final check.

5. Check the Y-axis in the same manner. (G0Y10) etc.

6. Set your speeds and acceleration. Go to Setup - Machine Settings Increase or decrease the maximum velocity allowed until the motor maximum at the bottom of the columns is at or below 7000.

7. Set the acceleration levels as high as possible without causing the drives to error out. There is one setting for rapid (non-cutting) moves, and one for cutting moves. The rapid will usually be set equal to the maximum velocity. The cutting acceleration will usually be around 4 to 6.

8. Make several rapid moves using the manual input box such as G0X20Y20 to move 20 inches in each axis, and then G0X0Y0 to return. If the drives error out and turn off, reset the number, lowering it, and turn the drives back on.

9. Dry run a program to check for cutting acceleration settings. To do this with plasma, simply turn off the cutting operation by de-selecting the box on the right that has a picture of a lighting bolt.

Running your first Cycle

Using the Main Production Screen

To begin, simply double click on the icon that was automatically placed on your desktop during installation to open the software.

Before cutting your first item, it is recommended that you Home the Machine.

To open an existing G-Code file, click on the button labeled Open.

To open an existing G-Code for editing, click on the button labeled Edit.

With the lightening bolt button UN-Depressed (this disables the torch). Click on Start Cycle to start the sequence. It should now run the file path, without actual cutting. Click on the lightening bolt when you are ready to make the actual cut.

This page left intentionally blank

Chapter

Machine Parameter Settings

Here we will cover all the settings related to the

Machine Parameter Settings of the Production Screen Setup Menu

Each area of the Machine Parameters section is separated by their tabs

· Machine Tab

· Inputs Tab

· Outputs Tab

· Tuning Tab

· Homing Tab

· Special M-Codes Tab

· Advanced Options Tab

· Torch Settings Tab

· Offsets Tab

· Joy Stick Tab

· Maintenance Tab

· Terminal Tab

· File Locations Tab

· Custom M-Codes Tab

Machine Tab

Comports

This version of Our CNC Plasma software will search all the Windows reported available comports and select the PC comports for you. If only two motors are found, then it is assumed that the Torch Height control is not available, and the software will switch to Oxy-Acetylene mode.

Buffer size

The maximum number of path points to be stored in each Motor. A buffer size of 16 path points is recommended. 18 is the max, 3 the minimum, but probably anything less than 14 will not work.

Max Angle

Maximum angle, in degrees, between tool path segments for them to be considered tangent. If the angle between adjacent line segments is less than this angle, and "Continuous Path" is checked, the path will be executed continuously without stopping. Lower values improve smoothness; higher values will reduce the overall cycle time. 30-45 degrees is a reasonable value. If you have checked the 'Slow at Vertex' box, then this angle setting is ignored, as the axis will automatically slow down at sharp angles.

Units

Select from Inch or Metric. This will tell the program that the scaling is in metric or inch. When the program encounters a change in G20 (inch)/G21 (Metric), it will make the correct math execution.

Motor Encoder PPR (pulses per rev)

Our motors use 2000 line encoders. Set this to 2000.

Work area Plus Limit+

Once the machine is homed, this is the maximum that the motors will travel. Movements or requests to move beyond this point will not occur, or will give an error warning. The "Max Limit" minus the "Min Limit" are the overall work area dimensions... Therefore it is possible to have Zero in the middle of the table, and work +/- 24 if you have a 48" axis. This most normally is a POSITIVE value such as 96 or 120 depending upon the table size.

Work area Minus Limit-

Once the machine is homed, this is the minimum that the motors will be allowed to travel. Movements or request to move beyond this point will not occur, or will give an error warning. This most normally is a NEGATIVE value. e.g. –0.10

Scaling (encoder pulses per inch)

Scale factors equal to the number of encoder counts per inch (or millimeter). If a positive number of encoder counts causes a negative motion in that axis, then change the scale factor to be negative. If your motor runs the wrong way, first change the sign of this number. There is a button with a “?” on it, clicking this will assist you in the calculation of the scaling value.
Example:
X=-15275
Y=15275
Torch=-10000
Slave scaling is probably the same factor as the master X, but could very well have a different "sign" either positive or negative, depending on how the motor is mounted. The slave to master ratio is a calculation based on the encoder line count and the scale factor.

Max Velocity

Maximum velocities for each axis in inches (or millimeters) per second. The value is the velocity used for rapid motions "G0 moves", and the smallest of the X, Y and/or Z-axes velocities is used as a limit on the overall feed rate during path moves "G1, G2, G3...” (If these values differ, it is up to the user to make sure that any programs do not exceed the maximum velocity of the slower axes.) Enter values in inches per SECOND; multiply by 60 for inches per minute.

Example:
X=15 (900 ipm)
Y=15 (900 ipm)
Z=5.0 (300 ipm)

Max Acceleration during Rapid and Jog moves

Acceleration values to use for each axis, in inches (or millimeters) per second. The value is the accel used for rapid motions "G0 moves", and when jogging. This can be from twice to even five times higher than the cutting accel rate…. Experimentation is recommended. A god starting value is the same value as the max velocity.12-15

Max Acceleration during Cutting moves

Acceleration values to use for each axis, in inches (or millimeters) per second per second. The smallest of the X, Y or Z-axes accels is used as a limit on the overall accel rate during path moves "G1, G2, G3". These values are typically much smaller than the rapid accel rates, and typically ¼ of the max velocity. 3-5

Max Motor RPM

As you change the Max Velocity and Scale, and Encoder Pulses Per Revolution, this value will give you an indication of the motor's RPM during the fastest move such a rapid "G0". This will help you to determine whether or not your motor will be over-revved, during rapid moves. Motor speeds of 8,000 rpm are guaranteed to fail… use good judgment here. Typically in a dual drive system, the slave motors cannot exceed 5000 rpm.

Inputs Tab

Each Motor in the system has 7 Ports. These are called ports because they can be either Inputs or Outputs. We have decided to use Ports B, C, D and G as inputs. All these ports are user programmable for a variety of different functions, including no function at all, where the input does nothing.

With 3 motors, each having 4 inputs, the system has 12 inputs available.

Other than Port B on Axis X, which we have dedicated to the Arc confirmation input from the Plasma Controller, each of the 12 input ports can be assigned to any of the functions defined in the drop down list. As an example, Port C on axis X could be defined as any one of several selection such as clicking on the E- Stop button, the Feed Hold button, the Start Cycle button etc.

If Port B or G on any axis is defined as a home switch, then that axis will home to a Limit Switch instead of a Hard Stop. If Ports C and D are defined as anything other than the End of Travel switches, then the SmartMotor is sent the UCI and UDI commands, preventing the Motor from shutting down when the switch is made. Otherwise, the UCP and UDM commands are sent restoring the EOT functions.

The selection for "Resume after M5x” where x=1,2... is an input assigned to a particular M command. If your program contains an M51 then it would pause the cycle until the input B on the Y motor was ON. This is helpful for times when you send an air cylinder operated Z axis down, and wanted to wait until it hit it's down limit switch before going to the next step of the g-code program.

DY is crash detector input and should be assigned as an E-Stop. CX is the E-Stop on the front panel of the control box. The P3 connector on the back of the control box is for extra E-Stop buttons, wire them in parallel.

When "Issue SM Command" is selected, a SmartMotor command should be entered in the text box, and the axis for the command should be selected. The SmartMotor command must adhere to the command structure and language of the SmartMotor version available. Try to avoid commands that will return a response such as RP (report position). For example, if you entered "MP D=2000 G" the SmartMotor will make an incremental move of 2000 pulses. This is an advanced function and for help, consult the factory.

Some inputs are outputs... We chose to use Ports B, C, D and G for Inputs. Animatics decided that Port C and Port G can also be used as brake control outputs. These outputs turn on when the motor thinks the motor brake should be engaged. There are two types of braking control. Failsafe braking is when the motor will turn on the brake whenever the motor has a failure and has a red light. Trajectory braking is whenever the motor stops moving, the brake will turn ON, and turn off when movement begins.

The Numerical display shows the status of the inputs and outputs of ports A thru G on each of the motors. The round circular indicators are Inputs. Inputs cannot be forced on by clicking on them, they are indicators ONLY. Putting the mouse pointer directly over any of the I/O indicators will display the user-defined name of the M-code or assigned input label in the Machine settings.

The rectangular indicators are Outputs on Ports A, E and F (in that order going down on the display). Each output is a user definable m-code. These outputs are turned on and off by m-codes instructions in your G-Code program, or manually by clicking on the rectangular indicator on the screen.

Outputs Tab

Each Motor in the system has 7 Ports. These are called ports because they can be either Inputs or Outputs. We have decided to use Ports A, E, F as outputs. With 3 motors, each having 3 outputs, the system has 9 outputs available.

We have dedicated M-Codes that can be used to turn on/off outputs. Each M- code output can be assigned to a motor output Port. In the example above, M3 and M5 are assigned to the X Axis - output Port A. In this case, issuing an M03 will turn ON the output port A on the X motor, and M05 will turn OFF the output port A on the X motor.

One of these outputs has been dedicated to the Arc Voltage input (that's right it's not an output, it's an input). That is Port A on the Torch (Z) motor. It is dedicated to sensing the arc voltage and cannot be assigned to an output. Please do not assign any m-code to Port A on the Z Axis.

If multiple m-codes are assigned to the same ports, then unknown results can occur. And only one of the outputs will be set, and it is unknown as to which one that might be. If you need a single M-code to turn on multiple outputs, then use the M14 or M15 commands.

Any text entered into the Description will show up as hint text when the mouse cursor is hovered over the rectangular indicator on the numerical display.

The Numerical display shows the status of the inputs and outputs of ports A thru G on each of the motors. The rectangular indicators are Outputs on Ports A, E and F (in that order going down on the display). Each output is a user definable M-Codes. These outputs are turned on and off by m-code instructions in your G- Code program, or by moving the mouse over the rectangular indicator and clicking.

The round circular indicators are Inputs. Inputs cannot be forced on by clicking on them, they are indicators ONLY. Putting the mouse pointer directly over any of the I/O indicators will display the user-defined name of the M-code or assigned input label in the Machine settings.

Homing Tab

Homing Order

Depending on the setup of the machine, you may want to home the axes in a certain order... It is recommended that Z be homed first for safety reasons, then Y and X. Enter the Capital letters of the Axis in the order in which they should be homed. In the typical application, this would be "ZYX". Enter only the Letters of axes that you intend to home. If you only want to home Z, then only enter Z.

Home Method

This is an indication of the homing method that has been chosen. If you chose an input to be a home switch, then Limit switch homing will be the method. If you chose NO input as a home switch, then hard stop homing will be the method.

Opposite Home Direction

The motors always home in the same direction. However, if these boxes are checked then the motor will home in the opposite direction than standard. This is helpful if you change the “scaling” from a plus to a minus, as the motors may now go to find home the opposite way. Once you have scaled the axes, and they are moving it the correct direction and sign, then start a homing process. If the motors go the wrong direction, then check this box.

Ignore Index Mark

Typically, you would home to a switch or hard stop, and then move backward to the index mark on the encoder. This will ensure the highest accuracy and repeatability of the homing sequence. This would place you within one encoder pulse every homing cycle. You have the ability to skip this extra move to the index mark, but you cannot guarantee the one pulse homing accuracy, you are left to the accuracy of your home switch. On systems that use the slave axis, you must choose ignore, otherwise, the two motors, master and slave may find the index mark at different locations.

Home Velocity

The velocity of the axis while looking for the home switch or hard stop is programmable. Drag the slider bar to where it homes smoothly. Hard Stop homing at a high speed would not be prudent.

Home Torque (Valid ONLY during Hard Stop homing)

This value is the amount of torque the system has to overcome in order for it to realize it has hit a homing hard stop. The minimum value should be 10 with a maximum value of 1000, NEVER, never use the max value. Start with an initial value of 120. The slave axis is typically a larger motor and will probably require a lower torque setting than the master, start with a value of 90.

Home Offset

This is a distance that after homing, the motor will move before it sets the home value. In certain applications, such as homing to a hard stop, it is not advised to have the "0" location against the hard stop. In this case you could offset the axis maybe 1/2" away from the hard stop and call that "0". Or you could leave this value at 0 and set the home value to be “–1/2”.

Home Value

The home value is the value stored in the servomotor AFTER it has found the limit switch or hard stop. Most system call G53 "machine" home the position that was found during homing... if you want to do the same, then leave the value here at zero. Otherwise set this value to the location that the axes are in when they find the home switch.

For example if you use the middle of the table as "0", but your home switch is at one end of the travel 48" total travel, then you could put "-24.000" as your home value. Or you could have this value as 0 and put in +24.000 as your Home offset above, and the machine will go to the switch located at –24.000, then move the offset amount (24”) and when it arrived there it would set the position to “0”.

The Homing Procedure

Hard stop homing The servomotor will move towards the end stop in velocity mode with limited current. Velocity mode means that the motor will travel at a fixed given speed. Limited current means that the torque applied to output shaft is current limited. (This current setting is adjustable by the user, from 10 to 1000, with 1000 being 100% of the available motor current). While the motor is in limited current mode, traveling towards the end stop at a fixed velocity, it is sensing the position encoder. When it sees the encoder has stopped turning, it assumes it has hit the hard stop, and immediately switches from velocity mode to torque mode. Torque mode just applies a force to the motor shaft, and ignores the position error that is associated with the velocity and/or position modes. This force will hold the axis up against the hard stop for about 1/2 second to allow the system to settle. Once it has settled, it makes a move it the opposite direction the "offset" distance. So if the offset was 1/2", it would have moved the axis 1/2" away from the end stop. At this time it will set the motors internal position to the "home value". If the home value was "0" then the motor's internal encoder will be set to "0". Homing is now completed.

But why would it home in the wrong place? If the limited current ("Torque") setting is too low, it will see the encoder stop rotating earlier than the end stop. This can be caused by a small piece of dirt in the track, a heavier than normal weight of the torch, or just general friction. This can be cured by slightly increasing the "Torque" setting.

Slave Homing: The same situation applies when homing with a slave axis. The difference is, the system waits for BOTH axes to hit the hard stops and switch to torque mode before reversing direction and moving out the offset amount. If the torque setting is too low, and the slave axis falsely finds home early, it will switch over to torque mode, thinking it need to hold against the hard stop while the master finishes it's move. But the torque mode can cause the slave to move faster than the fixed velocity of the master, and they will get skewed, possibly binding. This is true for the master axis as well. If the torque setting is too high, then the axis could jump teeth while holding against the end stop waiting for the other axis to finish.

Tuning Tab

WARNING - consult factory before adjusting these settings.

K Proportional

Proportional gains used by the PID in the motor. Try 50 as a starting number

K Derivative

Derivative gains used by the PID in the motor. Try 200 as a starting number

K Integral

Integral gains used by the PID in the motor. Try 15 as a starting number

K Accel Feed Forward

Acceleration Feed forward used by the PID in the motor. Default = 0

K Integrator Limit

Integration limits used by the PID in the motor. Try 100 as a starting number

Error Limit (Following Error limit)

Position error limits, in encoder counts, used by the PID in the motor. (usually 4000-8000)

Sample rate

Usually a value of 1

K Velocity Feed forward

Velocity Feed forward gains used by the PID in the motor.

K Gravity

Compensation for gravity. This makes the gain stiffer during acceleration when lifting and makes it stiffer when decelerating on a downward move. We suggest you leave this at 0.

AMPS value (1-1023)

This is the percentage of the max current allowed to the motor. 1023 is 100%, while 1 is 0.1%

Additional Parameters

There are parameters such a "F=8" which will be sent to the motors during the setting of the gains

Special M-Codes Tab

M86 ... M91

These m-codes will play a sound file when they are encountered in a g-code program. If a sound file is to be played, use the browse button to locate the file, (“WAV” files only) and then check the “enable” box. If you want the program to hold up any further executions until the sound file has finished, click on the “Wait for completion” checkbox. If you have no sound card in your system, and you choose to enable any M86 thru M91, you can expect an error from Windows.

M80 ... M85

Consult the factory for the Issue SmartMotor Commands...

There are occasions when you want an M-Code to perform a function that talks directly to the SmartMotor. In these cases, these m-codes can be configured to issue Smart Motor commands. These M-Codes are dedicated as M86 thru M91. To send a Smart Motor command, enter the code in the text box exactly as the SmartMotor would expect it. Avoid commands that return a response (such as any report command.) Also, select the axis for which the command is intended. As an example, "AMPS=205" will set the torque on all the selected axes to 20.5% of the motor's maximum continuous torque.

Advanced Tab

Ask to Home at startup

Selecting this will bring up a pop up window asking if you want to home the motors at start up of this program. It is recommended that you ask to home at startup. Default is checked

Show User Defined M-Code Button

A button will be enabled on the main screen that will issue M-Codes when selected and de-selected. The M-Code that is issued is defined in the following text boxes. If you want to have a button on the screen to turn On and Off some output, this would be a convenient way to do that. Default is M60 and M61, and it is checked.

If no Feed rate is set, use this default value

When checked it will automatically use the defined feed rate if the G-Code file failed to have an “Fxx” feed rate defined. Be sure to fill in a value for the default feed rate. Default is checked with a value of 100 in/min.

Allow Re-Zeroing in G53 (machine coordinates)

Normally, it is not possible to change the zero that was set by the machine during a homing procedure. Selecting this box will enable the "Zero" button on the screen to be present when you are in G53 mode. This will change the machine reference, use with caution. Default is unchecked.

Keyboard character turns on / off an output

If you would like an output(s) to turn on/off by pressing a key on the keyboard, this will allow you to do that… Be careful, some keys are used to start a certain function… such as “r” is the same as clicking the “Start” button. Click on the “?” button for help determining the number that should be entered here. The default value is 0

These Outputs turn OFF when the Servo Errors

These output(s) will turn off when the servo motor errors, or is turned off for any reason. Click on the “?” button for help determining the number that should be entered here. The default value is 7

Feed Hold Turns these Outputs OFF

When selected, it will turn off all of the outputs that are selected. These will turn off when the “Feed hold” button is clicked. Click on the “?” button for help determining the number that should be entered here. The default value is 7

Resume turns these Outputs ON

When selected, it will turn ON all of the outputs that are selected. These will turn on when the “Resume” button is clicked. Click on the “?” button for help determining the number that should be entered here. The default is unchecked value of 0.

Wait for M50 before resuming (Input port B on X axis)

Discuss this use with us, it is custom for those who wish to use their own THC. After clicking Resume during a Feed hold condition, the program will wait for an input (XB) to be true before moving the XY motors. The default is unchecked.

Do not reset line number when clearing E-Stop condition

When selected, the g-code file will maintain the current line number. This is useful in restarting a program, from the place it last stopped, due to an E-Stop. The default is checked

Start Cycle with Line Number >1 forces these Outputs ON

As an example you could use M60 to turn on your exhaust fan. Normally the M60 command would appear at the beginning of the G-code program. If you start the program from somewhere in the middle, (a line number greater than 1) the M60 command is not read, and hence not acted upon. This option allows you to turn on an output, such as the exhaust fan, when you start the program from the middle. The default value is 0.

M30 (end of program) turns these Outputs OFF

This will turn off all of the outputs that are selected. These will turn off when the “M30 (End of File)” code is read in the file. Click on the “?” button for help determining the number that should be entered here. M02 is also an End Of File indicator, but it does not turn off any outputs. The default value is 7.

Zoom All if rapid move exits the current zoomed in screen

In the case where you have used the zoom to get a closer look at the object on the cutting table, this will zoom out to the complete table if a rapid move takes the torch outside of the zoomed-in viewing area

Vector Slow Proportional Up To XX.X Degrees (89 degrees max)

As you approach a location where the path will make a sharp angle and you are in Continuous Path mode and have Slow at Vertex selected, the system will slow all the axes in order to make the move smoothly. The amount it slows down is based on the size of the upcoming angle. If the angle is one degree, the slowdown is virtually non-existent. As the angle reaches 30 degrees, you will begin to notice it slowing, and at 85 degrees, it creeps very slowly through the corner. As you experiment with this value, you may find that the slow down at 55 degrees is slow enough to make a 90-degree corner smoothly. If that is the case, then set 55 as your value here, and any turn greater than 55 degrees will only slow down to that speed. Speeds at angles less than 55 degrees will slow down proportionally. This amount is usually set after you are satisfied with your selected velocities and accelerations in the machine settings, because they will affect this. Experimentation may be necessary. Default is 60 degrees.

Continuous Path

When checked, this will force the interpreter to join all the lines and arcs into one continuous path. This program has the ability to "look ahead" and merge line segments and arcs that are tangent, (as set by parameter 'Max Angle') into a single smooth motion without stopping at each end point. Selecting the Continuous Path checkbox will enable this feature. The Max Angle parameter, as defined in the Machine settings tab, specifies the maximum angle, in degrees, between line segments for them to be considered tangent. Continuous Path can be turned on and off while a program is running using M-Codes M21, M210 and M22. The default is checked.

Example:

M21 turns on Continuous path

M22 turns off Continuous path

Maxang can be changed in the program by M210 Px.xx (where x.xx=max angle)

Example:

M210 P65.0 (sets continuous path ON with the Max angle at 65.0 degrees)

Slow at Vertex

When checked this will slow the axes down prior to a change in the angle at the next vertex. The amount the plasma cutter slows is proportional to the tangency angle of the next vector. The default is checked.

When Continuous Path is used with Slow at Vertex, it allows the path to be continuous and the speed at the non-tangent corners to slow down proportional to the upcoming angle. This slow down amount is proportional to the cube of the cosine of the angle. For instance, the cosine of 60 degrees is 0.5, cubing it becomes 0.125, this is multiplied by the present federate, and the vector speed slows to this amount. If the vector speed was 100 ipm then the speed as it rounds a 60-degree corner will be 12.5 ipm. Since the cosine of 90 degrees is 0, the motion would slow to zero speed and NOT continue, a big problem here. Since we are using the cube of the cosine, an angle above 84 degrees will slow to 0.001, or one thousandth of the present speed, which proceeds very slowly around the corner. Please select a value starting at 55-60 degrees and going up or down 2-3 degrees at a time to find a value that allows smooth motion in sharp corners. Remember that acceleration and maximum feed rate play a part in the smoothness also. Experimentation would be helpful here. When using the Slow at Vertex feature, the MaxAng value of continuous path is ignored.

Slow at Vertex can be turned on and off while a program is running using M- Codes M23 and M24.

Example:

M23 turns on Slow at Vertex

M24 turns off Slow at Vertex

With Continuous path turned on, there are several conditions under which the programmed tool path will be broken into separate motions:

1) Two consecutive tool paths are not tangent (greater than MaxAng and Slow at Vertex is NOT checked.)

2) A rapid motion (G00) is encountered.

3) A dwell command (G04) is encountered

4) A feed rate change is encountered. (e.g. F20)

5) Any M-Code is encountered. (e.g. M05)

6) A subroutine jump (e.g. M98)

7) A repeat command (e.g. G76 L2 P10)

When one of these conditions is encountered, the previous motion will decelerate to a stop before the next motion will be started.

Allowable Overshoot:

This has to do with the software limit switches. In most cases, the software limit switches will not allow a movement past the soft limits. However, if you attempt to drive the axes to the limit, they may overshoot due to poor tuning. This amount allows you to be a little forgiving, prior to shutting down with an error. Default is 0.010”.

Minimum arc radius allowed

This is an information box, depending upon your scaling of pulses per inch, or millimeters, you will not be able to perform an arc with a radius less than what is listed in this box. You cannot change the data here, it is only for informational purposes.

Max allowed comm errors before alarming

This will ignore the sequential communication errors up to the quantity that is set. Once the count is equal to the value, an alarm message will be posted. The default is 1, and should be left there… Only increase this if you have a noise problem and you are trying to debug it.

E-Stop abruptly halts motors instead of decelerating to a stop

This should remain unchecked. This will slam the motor to a stop. While doing so it will draw all the power it can from the power supply. Each motor could draw up to 12 amps; two motors can draw 24 amps. This is usually enough to send the power supply into an over-current condition which will cause it to shut down. Unless you have a 30 amp power supply (typically we supply 10 amp units) you should not check this box, and only check it if you need to slam to a stop.

Use APS (automatic proportional slowdown) for short segments

Selecting this check box will force the G-Code interpreter to examine the upcoming path segment. If the segment is smaller than a certain size, it will proportionally slow the feed rate down automatically. Path lengths less than X.xxx in length will be slowed down, but not less than Y.y% of the defined feed rate. Other lengths will be scaled proportionally up to a length of Z.zzz.

Let's imagine that X.xxx = 0.785"

and that Y.y% = 25%

and that Z.xxx = 4.0"

and the current feed rate is F120 (120 ipm)

Now let's look at an example. A small circle with diameter of 1/4 inch, has a path length of Pi * 0.25 = 0.785" This will force the CNC to limit the feed rate for this, or any segment shorter than it, to run at of 25% (Y.y%) of 120 ipm which is a feed rate of 30 ipm. Segments with lengths greater than the minimum 0.785, will be adjusted proportionally up to the length of 4.0". So a circle with the diameter of 1.0" has a path length of 3.14", it is greater then 0.785 and less than 4.0", so it's feed rate will be scaled proportionally. It will be scaled between 25% and 100% of the programmed feed rate, it this case it will run a 1" diameter circle at a feed rate of 80% or 96 ipm. Once the segment length is greater then 4.0", the feed rate will remain at 100% of the programmed feed rate, or 120 ipm in this example. Experimentation would be helpful here.

Freeze THC during these short cut paths

Selecting this will force the THC to hold at the Pierce Height and is inhibited from any movement during the cut.

Show Sub-Routines in G-Code Box

Selecting this will make the G-Code window smaller so that the subroutine window will fit below it. If you are using subroutines, select it, if not leave it unchecked.

Enable View option - Show Positions

Selecting this will enable the drop down menu on the main screen "View" to contain a selection for showing positions. This will display the time delta and encoder positions to which the motor is going. This function is best used for troubleshooting.

Ghost Image Color choices (cutting / rapid)

When you first open a tap file to cut, the image is drawn on the screen. (the ghost image). The colors of this ghost image can be selected by the user for both the rapid moves as well as the cutting moves. This is just a matter of personal preference.

Cutting Path Line Thickness and color

When the system is cutting, the path is drawn on the screen. Here you have the ability to select the color of the line (click anywhere in the white box). You can also choose the thickness of the line; a thicker line will show up easier when viewing from the other side of the machine. This is just a matter of personal preference. Why would I not see the path being drawn? Under the View menu on the main screen, be sure to have "Show 2D Path" checked.

Numeric display color

Click on the example, and you can choose a color other than the default yellow.

Torch Tab

Scaled arc voltage input

Some Plasma system can deliver a low (<10volts dc) voltage proportional to the arc voltage… In our standard system, we scale the 0-300 volt arc voltage down to 0-5 volts…. In the case where the plasma supplier can deliver the lower voltage signal, it may not necessarily be 5 volts=300volts, please enter here the voltage that they can supply. One plasma supplier we know uses 0-6 volts for the 0-300 volt reference. In this case you would put 6 in the text box. The default is 5.

Down force used when searching for the plate

This is how much force the motor is allowed to apply while it senses the following error of the encoder, hence sensing that motion has stopped.. Keep this number small, especially for thin material. 80 to 100 is the default. These values represent 8% and 10% of the motors continuous torque rating.

AVC Height sensing delay (0.25 to 2.0 seconds)

This is the settling time after the arc has been ignited and movement of the gantry begins, before we allow the AVC to make it’s “height correction”. The initial arc is unstable for the first ½ second or so, and if the AVC was allowed to make corrections it could jump erratically based on the unstable arc. This ¾ second delay, allows the arc to stabilize before we start the correction. Default is 0.75 seconds. If a pierce delay is used, it will be added to this value automatically by the system.

Arc output ON delay in CPU cycles (4069 CPU CYCLES IN ONE SECOND)

When cutting VERY this material (0.025”), it is possible that the arc can burn away all the material and extinguish itself before the gantry even starts to move. There is a sequence of events that occurs when the arc initiation takes place. First the AVC sends a command to the plasma unit to “turn on the arc”, once the plasma unit determines that the arc is on, it sends a signal to the XY motors saying the arc has been established. It is then that the gantry begins it’s movements, and this exchange of signals can be a small delay in time. During that delay, the thin material can be burnt away completely and the arc goes out. This feature, will delay sending the “turn on the arc” for a short amount of time. This delay can be tuned to have the arc established at the exact time the gantry movement starts it’s move. This feature ONLY works if the “E-Stop on lost Arc” is UN-checked. (this checkbox is located below the arc voltage/arc set- point display). Why is this necessary? It is because we are beginning Gantry movement without arc confirmation; otherwise we would go into an E-Stop condition as soon as we lost the arc. Normally we would not begin movement unless we have confirmation that the arc is established. In this case it is assumed the arc will establish itself and we should just begin movement. This delay allows us to begin movement, which takes some milliseconds, and then turn on the output to ignite the torch. The value here is in CPU cycles of the intelligent motor. This will be a more accurate and more precise value for the delay. The CPU of the motor makes 4069 cycles per second. If you enter a value of 800, it would be 800/4069 = 0.197 seconds. The default value is 1.

AVC Correction Sensitivity Factor

This is the GAIN of the AVC. This factor (a multiplier) sets the correction speed of the AVC. If the value is too low, the AVC will be slow to make corrections, if it is too high, the AVC will overshoot when correcting and become unstable. Typical values are between 10 and 20.

AVC # of Measurements to Average

Typically when you read an analog value, it is best to take several readings and then take the average of those readings. This eliminates spurious noise related measurements that are anomalies that cause erratic jumping of the AVC. Dynatorch has two versions of the electronics that are in the AVC control box. The earlier versions required that we take about 75 measurements and average those prior to making a decision on how much to correct. The current electronics allow us to take 5 to 10 measurements. This gives a much, much faster response time. And this makes a smaller and smoother correction. Basically instead of a 3-4 corrections per second, it can now make 20-25 corrections per second. Because there are those customers with the old electronics out there, the default value is 75, but if you have the new electronics (starting around May 2005), you can use a value between 5 and 15. You should also lower the correction sensitivity if you have the newer electronics.

Fixed distance jogging with the torch

The X and Y-axes can be setup for “fixed” jogging. It is possible to fix the jog amount to 5.0” or even 50.0". Every time you click on X or Y the axis will jog 5.0”…. Well if you have the fixed jog selected and you attempt to jog the Torch 5.0 inches, it’s will crash, since it only has 4” of travel. Rather then prevent the torch from making fixed jogs, we allow you to set the value of a fixed jog for the torch here. So each click of the torch Up/Down button during "Fixed" jogging will more the torch this value. The default is 0.0625” (1/16”)

While cutting, each click of the torch jog button will move

Holding down on the Jog button will cause a buffer underflow in the X and Y motors. By just sending a quick instruction of "Move this amount" to the torch, we eliminate the buffer underflow problem. The default is 0.0625” (1/16”)

Number of seconds to wait for the arc to establish before it is an error

In previous versions of this program this delay was fixed at 4 seconds, but recently some plasma units are requiring up to 5 or 6 seconds from the time we send the signal to ignite until they actually do. This was causing us to timeout just as the system was igniting. We have now made this value adjustable by the operator. The default is 5 seconds. If, from the time we send the signal to ignite the torch, and we wait 5 seconds without the arc confirmation, we will consider it an error and shut the system down.

Delay time after arc is established and before starting gantry movement, for arc to pierce thick material

Thick material, 3/4" to 1.0" may take an extra second or two to pierce thru the material. We will wait this time before beginning the gantry movement to allow the pierce to complete. The default is 0. If you do not want to change the settings for each different part, you can do it is a G-Code program by setting M25 Px.xxx. The P word is used to set the delay time. Be sure to reset this value to 0 when cutting thinner material.

Raise the torch between cuts in OxyFuel mode

This checkbox enables the torch to rise between cuts in the OxyFuel mode. Typically when the system is used with the plasma torch, the torch lowers itself down to touch off on the material, and then it rises up to the pierce height. But with Oxyfuel torch, doing this will most likely extinguish the flame. Therefore we expect the customer to jog the torch down to the preferred cutting height manually, and set the cut height using the button just above the delay timers for preheat and pierce. Once the height has been set, it is memorized for the entire cycle. If this checkbox is not checked, then the torch moves between cuts at wherever it currently is set, it will not raise or lower unless the jog buttons are used by the operator. If this checkbox IS checked, then the torch raises to the home position between cuts. When it arrives at the next cut, it lowers itself back down to the cut height position that was set by the "cut height" pushbutton. The default is checked.

Using Jog buttons during a cycle will re-teach the cutting height

If you jog the torch up or down during a cut (using the Torch Up/Torch Down buttons) then the memorized cut height position is re-memorized. The current down position that is memorized is displayed in a textbox that shows up next to the set cut height button. This is useful if you need to make a height correction during a cut. The default is checked.

Pause at pierce height before going to cut height for preheating

In an OxyFuel cycle, the torch will lower itself to the cut height while the preheat and pierce delays time out. However if this box is checked, then it will pause on the way down, at the pierce height above the cut height. The pierce height is the ?/16ths value. This will perform the preheat from the pierce height and then make the pierce at this same height, once the pierce time has expired, the torch will lower itself to the cut height to complete the rest of the cut. This should prevent any splash back that may clog the torch tip if it was to pierce at a lower height.

This output turns ON for OxyFuel Cutting Oxygen

You can determine the output you want to turn on the cutting oxygen valve. Default is 2

This output turns ON for OxyFuel Preheat Gas

You can determine the output you want to turn on the preheat valve. Default is 4

Leave preheat gas output on between cuts

Some systems cannot turn off the preheat between cuts or the torch may extinguish. This will allow the preheat to stay on until the cycle is completed. Default is unchecked

Offsets Tab

Service and Load Positions

These locations are based on the homing location of the machine. They are relative to where the machine found home. They are NOT based on the floating zero locations. If you have a 48" x 96" machine, and jogged to the center of the table, then clicked Zero All, even tough the numerical displays will show 0,0, the machine knows where it really is in respect to the home position. So if you click on the Service position, it will do the necessary math required to get the machine to, in the case above, X0 and Y48 based upon where it found home.

0,0 Position

This location is NOT and I repeat NOT based on the homing location of the machine. It is the position based on the current numerical display values. AND pressing the "0,0 Pos" button DOES NOT require homing! So be careful.

Raise torch first when "Service pos" button is pressed

Raise torch first when "Load pos" button is pressed

Raise torch first when "0,0 pos" button is pressed

The check boxes will force the torch to raise to it's home position completely, prior to moving the X or Y axes.

G54... G57

These dimensions are the offsets from the homing position on the machine. The homing position, also known as the machine reference, is G53, and is relative to the physical home 0,0 location after the machine has done a homing routine. If you would like to work in an offset mode, enter the locations from the machine home here. In the example, if G54 was entered in the G-Code, and a G0 to X0Y0Z0 was performed, the machine would move to x=0.5 y=0.5, z=0.0 but the display (when in program) will show x=0.0, y=0.0, z=0.0. You can choose to jump between the four offset coordinates (G53, G54, G55, G56, G57) at any time. The G54 is your typical program home location. It is offset from the machine home by some distance. In fact, when the machine first finds the machine home it then switches to G54 mode. Issuing a G10 will immediately reset the present coordinate (G54 thru G57) to 0,0,0. However, it will not reset the G53, machine home position. Issuing a G92, followed by a X10 or other Axis and position will immediately set the present location to X=10.

WARNING In this program G53 is MODAL.

Joystick Tab

To activate the joystick, go to the Setup pull down window. Go to Machine settings. Go to Joystick Tab. The window you arrive at should look as follows:

Enable the Joystick

This check box is to enable the Joystick; this will be grayed out if Windows does not find any joystick connected to it. When in doubt, go to the Windows Control Panel and look in the Gaming Options for the joystick / game pad devices. From the control panel you can also test and calibrate you joystick.

Reverse X Dir

This checkbox will reverse the direction of the motor. If when you push the joystick to the right, and your torch goes to the left, it would be suggested that you change the state of this checkbox.

Reverse Y Dir

This checkbox will reverse the direction of the motor. If when you push the joystick to the up, and your torch goes to down, it would be suggested that you change the state of this checkbox.

Use velocity mode for freehand joystick. The freehand joystick is the one on the LEFT

The joystick normally operates in torque mode. When the stick is centered it give no torque to the motors, when it is pushed off center, the torque to the motor (corrected for direction) is increased moving the torch. If you are not paying attention and you run the torch to the end stop, and if it is in torque mode, it just applies a force against the end stop, but does not get a following error. Releasing the stick at this point reduces the torque to zero and the motor just sits happily with no torque applied.

However in Dual Drive Systems, if the axes have any mechanical misalignment, then the master is free to move at will because there is no torque on the motor, but this misalignment can cause the master to move, and this in turn will force the slave to move because it follows every single encoder pulse the master moves, and what happens is the slave, while compensating for misalignment, is pulling the master who is rotating and sending pulses to the slave to follow the master and it is a vicious circle. And the system will walk it way all the way down to the other end of the table. So for these systems, we have this checkbox that puts the motors into velocity mode where they have torque on them all the time on order to maintain position. Bt what can happen here is any move that causes the system to hit something can cause a following error and shut the motors down. So be careful.

Maximum freehand cutting speed

The freehand cutting joystick's speed can be limited. For those who do not want the joystick so sensitive to high-speed moves, they can limit the torque/speed with this slider control.

Joy Stick Buttons

Each button on the joystick is numbered. The function of each numbered button can be found by clicking on the joystick buttons and viewing the indicator that lights up. NO movement will take place while the joystick setup screen is opened.

Joy Stick Button #12

Button on the joystick is used to turn on/off an output(s). Select the number with the help of the ? button.

General Joystick Notes:

Our cutting system is equipped with a uniquely flexible joystick that allows the user to have almost complete machine control in a portable, hand held device. Normal G-Code cutting operations, jogging (X, Y, and the Torch axis), speed controls, canned and gantry relocations are all available to the user by the joystick use. In addition, the joystick gives the user a freehand (non G-Code) cutting control tool.

The system utilizes a Logitech Dual Action Game Pad (or compatible) as the control device. It is available through us or from most electronic stores, retail outlets. The joystick plugs directly into an available computer USB port. The joystick's working distance from the computer can be extended by employing a standard USB extension cable also locally obtainable. Be sure to install and test the joystick under Windows prior to attempting to use it with the CNC software. This can be done under the game controllers in the control panel of the Windows operating system.

Joystick Use

To activate the joystick click the radio button labeled joystick located under the jogging speed slider control on the main software screen. If it is not visible, then you have not enabled the joystick on the above settings page.

The left joystick controls freehand jogging operation. The further away from center you move the joystick the faster the torch will move. Pressing down on the left joystick while it is off center will result in a doubling of speed (torque).

Table limits are NOT in effect while using the joystick, caution must be observed so as not to run into the X and Y hard stops.

Straight Line Cutting

The right joystick only is used for straight-line cutting. It operates in a similar manner to the left joystick but only runs at a fixed speed curing a G23 while the torch is down and ignited.

Familiarize yourself with the location of buttons 8 and 6.

If a G-Code file IS presently loaded the joystick cutting operation speed will default to the G- Code initial cut rate modified by the feed rate percentage window. For example: If the G- Code initial rate is set to 120 inches per minute (F120) and the feed rate window percentage is set to 50% the resultant freehand cutting speed will be 60 inches per minute.

If NO G-Code is loaded presently, the cutting speed is defaulted to 100 inches per minute and modified by the feed rate percentage window setting. For example, if the feed rate window is set to 75% the resultant cut speed will be 75 inches per minute.

With joystick cutting you must emulate manually the operations done for you automatically by G-Code. For example:

·Start cut cycle

·Send torch in a direction to cut.

·Stop cut cycle.

To complete a freehand cutting operation do as follows:

1. Position torch over where you wish cut to begin with the left hand joystick.

2. Press button number 8 to start cut cycle, this issues a G23 to the controller.

3. As soon as the arc is established, move the right joystick in a direction you wish to cut. You can be pushing the joystick before the arc has struck, but it will not move until the arc strikes.

4. When reaching the point you wish the cut to stop release the joystick and quickly press button number 6, or just press button 6 and the joystick will stop when the arc goes out.

5. The arc will terminate and the torch will retract to it's home position.

Should you run the torch off the edge of the material or into a hole the arc will terminate and an emergency stop will occur. To clear this condition press button number 10. This clears the emergency condition. Then press button number 6 to complete a normal stop cycle.

Maintenance Tab

Query Motor Information

The CNC cutting system has 2 or 3 servomotors connected to it. This tab allows the user to query the motors for some information such as serial and model numbers

Erase Program in Motor(s)

The motors have a program in each of them to offload some of the burden from the PC for more efficient control. (They are intelligent motors). There may be an occasion when the factory requests that you clear the program from the motor (like a re-install). If this is the case, you will be instructed to open this page and click the clear the motor program. Once they have been cleared, you must close this program, otherwise expect lots of communication errors as the PC tries to ask the motor to perform an operation for which the motor no longer has the program. When the PC program restarts, it will download fresh programs to each motor and restore everything in it's proper order and be ready to begin work again.

Terminal Tab

This tab will allow the operator to directly communicate with the motors. It will also give a quick diagnostics of the current condition of the motors. The data in" (E99999)" is the serial number of the motor.

Send to

Commands typed into the command line will be sent to either All motors, or a specific motor. You should understand the command structure of the motors before sending instructions. In the example above, "RP" command was sent to all the motors. The Response was the current encoder position of each motor it found. Likewise the command "OFF" would have turned the motors off, "G" turns them back on again, not "ON" as you might assume.

Current motor information

State: Is the motor ON or OFF ?

Position: The present encoder position of the motor.

Follow Err: the present following error of the motor (it should be 0 or 1)

I/O A ... G: the status of the ports A thru G

1 = no input/output active

0= input is active/output is ON

Bus Volts: The voltage on the pins A1 and A2 of the 7 pin motor connector.

(the power supply voltage)

Current: The number of amps the motor is currently drawing

Temp degrees C: The internal temperature of the motor.

These motors shut down automatically at 70 degrees.

Status: A code that describes the present motor status or error condition.

See the motor manual for a complete list.

AMPS: The current limitation of the motor.

Max current is 1023.

If the value is 512 the motor has been limited to 50% of its current draw.

Mode: The current mode of the motor.

Version: The firmware version of the motor.

Analog: The 0-5 volt input from the arc voltage scales from 0 to 1023 units

Slave Encoder: The current external encoder value of the slave axis

Continuous update and refresh:

These control the refresh of the current motor information.

Files Tab

This tab will allow the operator to decide where the files should be opened from and saved to. Clicking on the browse button will allow you to search for the directory (folder) you would like to use.

File Open Extensions

List the file extension you want to filter when you open a G-Code file. Do not add the "." (dot). Only files with those extension will be filtered through and show up.

The defaults are TAP, NC, and TXT. Bt you can add any others you like such as CNC, or whatever your G-Code converter uses as it's extension.

Custom Tab

This tab explains custom M codes that were developed for certain applications. These are typically an instance where the end user wanted a special feature and we added it to the program. If there are special settings pertaining to the custom M code, they can be filled in here.

Chapter

The Main Cutting Screen Controls

This section contains the descriptions of the Main screen elements

· The Menu Options

· The Numeric display

· The Jogging Buttons

· The Start Buttons

· The Go To Position Buttons

· The Plasma OxyFuel Buttons

· The Visual Cutting Area

Menu Options

Under File:

Open G-Code File

This opens a dialog box for selecting a G-Code file. The file filters are pre-selected by the user on the Advanced Setting page under Machine Settings. The selected file is loaded into the Interpreter. If the immediate folder that opens is not the current program folder, right click on the desktop icon that started the program to check the properties. If there is nothing in the “Starts in:” text area, then add the path to the program folder in the text area.

Edit G-Code and New G-Code (sub) Bank and New Subroutine

These selections open a dialog box for creating a .tap G-Code file, or for editing an existing one. The selected file is loaded into the edit window. The file can be manipulated here and Saved, Saved As, Saved and Opened To save an unaltered version of the file, click the Cancel button.

New G-Code (sub) Code Wizard

This selection opens the code wizard for building simple shapes like circles, rectangles, gussets and bolt circles (even arrays of these)

Save

Choose Save to store the file you are currently working on. It will automatically keep the same file name the file had when opened, and will store to the same location as where the file was residing when opened.

Save As

Use Save As the first time you save a new file, or to save a second copy of a file, giving it a name such as “sunmoon2.tap”. Use Save As to save a copy of the file with the original name to a new location, such as on your desktop or to a zip disk.

Convert DXF - G-Code

This opens the DXF Converter for converting two dimensional .dxf files to G-Code. See DXF Converter for more information.

Exit Program

This will exit and close the program window.

Under Setup:

Manually Set Home

This will allow the operator to set home manually; it operates the same as if the machine had run its search for home routine. The assumption is that the present location of the axis truly is the home position.

Search for Home

This will home one or all the axes, in the Homing order that was selected in the Homing tab of the machine settings. The homing style, whether Hard Stop or Limit Switch, will depend on the selection made under Machine Settings, on the Inputs and Homing tabs.

Clear homed flags

This removes the "H" or "Axis is homed" bit and sets it to false. This could be useful if the system homed in the wrong palace and now won't allow you to jog back closer to the home switches. By resetting the homed flags, you can jog anywhere because there are no limits when the system is not homed.

Machine Settings

This will open the Machine Settings tab. These settings control and setup the basic machine parameters etc. See the Machine Settings section for complete descriptions.

Under SmartMotor:

This will allow you to go Online and Offline in communicating with the motor. This is the same as the Connect and Disconnect buttons.

Under View:

You must check the Show 2D Path drop down if you want to see the path drawn on the screen while it is cutting. The color and thickness of the path lines are user selectable in the advanced tab of the machine settings.

Under Help:

About

This provides software version and copyright information.

Opens this Manual. This opens this help file.

The Numeric Display

Plasma display

Oxyfuel display

ALL ON button

This is a very important button. Whenever the drives turn off due to an error of any kind, the ALL ON button will restore machine operation. This is used after E-stops also. Whenever the drives turn off, the readout numbers will go GRAY to indicate that the drive is off-line. The readouts will still operate and indicate actual machine position even if pushing the machine manually turns the drives. Clicking on the ALL ON will restore the drives to on-line condition and all drive coordinates will return to YELLOW or what ever color you have selected in the advanced settings. See also Axis Label check box below.

Axis label Checkbox (X,Y,Z)

When checked, this will turn the power ON to the Motor and it will servo in position. De- selecting the box will turn the motor OFF, it will be free to turn by hand, but the encoder will maintain the correct position.

Status Error Indicators:

The area below the axes numerical display is the status area. If an error occurs, the error text will turn red, indicating which error occurred. To clear a red error indicator, click on the status area. If the indicator does not clear, the problem still exists. The errors are “OFF” when the motor is off, “POS ERR” when the motor has a following error, “OVER CURR” when an over-current condition has been applied to the motor, and the “TEMP” when the motor is overheated greater than 70 degrees C.

The Master Slave Button (M and S on the button next to the X numeric display)

This button will toggle between the servo position and information of the Master or Slave on the dual drive axis systems. In the above photo, there is NO slave motor so the slave "S" has an X thru it.

Coordinate systems

The numeric display always shows positions in program coordinates, NOT machine coordinates. Because you may wish to re-assign the 0,0 point in order to cut a pattern somewhere out on the table other than the lower left corner, you can re-zero the coordinates anywhere the machine is at any time. The display will not affect the machine limits or rapid positioning buttons at the bottom of the screen.

The Numerical display also shows the status of the inputs and outputs of ports A thru G on each of the motors.

The round circular indicators are Inputs on Ports B, C, D and G. Inputs cannot be forced on by clicking on them, they are indicators ONLY. Putting the mouse pointer directly over any of the I/O indicators will display the user-defined name of the M-code or assigned input label in the Machine settings.

The rectangular indicators are Outputs on Ports A, E and F (in that order going down on the display). Each output is a user definable M-Codes. These outputs are turned on and off by m-code instructions in your G-Code program, or by moving the mouse over the rectangular indicator and clicking.

The Jogging Window

X- X+ Y+ Y- Buttons

These buttons allow the individual axes to be jogged. The Jog Speed bar adjusts the speed of the jog. Full speed is approximately one half of the maximum velocity as set in the Machine Settings.

Continuous

If Continuous is selected, the axis will jog continuously while the button is held down, and stop when it is released.

Fixed

If Fixed is selected, each click of the button increments the axis in the amount entered in the fixed text box. Negative numbers are not allowed, jog in the reverse direction if you want to go negative.

Keyboard Jogging

All jogging functions are also available from the keyboard if this check box is selected. The keyboard arrow keys control the X an Y axes

STOP

The Stop Button (with the stop sign) will appear only in the Fixed jogging mode.

Joystick

This radio button will allow the jogging to be controlled by the Joystick. Please see the machine settings for the button usage of the Joystick. We recommend the Logitech game pad available at most department stores for less than $20. We have also tested the Wireless version of the same joystick, and it worked well without the plasma ignited… We have not yet tested the wireless functionality with the plasma ignited (there could be a noise issue). You can cut with the joystick. Windows must detect a joystick attached to the PC for this radio button to appear. For more information, see the Joystick section.

Torch + Torch –

These buttons allow the torch to be jogged. The Jog Speed bar adjusts the speed of the jog. Similar to the XY jogging arrows, full speed is approximately one half of the maximum velocity as set in the Machine Settings.

If Continuous is selected, the axis will jog continuously while the button is held down, and stop when it is released. If it is during a cutting cycle, the torch jog will be limited to the fixed increment that was set on the torch tab of the machine settings.

Fixed torch jogging is also set in the machine settings under the torch tab. Since the torch has only 4" of travel, if you wee to select a 12" move for the X or Y and forget to deselect the fixed button, then the torch would move to where it should never go.

Torch CUT / No-CUT and THC (height control)

THC AND PLASMA THC AND PLASMA

SHOWN ON SHOWN OFF

Just below the Torch up and down jog buttons are two buttons for controlling cut and dry run as well as THC (torch height control for plasma only). If the lightning bolt button is depressed, then the machine will cut when running a G-code program using whichever process (plasma or oxy) was selected above. If the lightning bolt button is not depressed and gray, then no cutting or THC will operate. This includes the initial pierce height sensing operation for plasma. The Lightning Bolt button controls the torch, either plasma or oxyfuel. If the lightning bolt is NOT depressed, neither torch will activate.

If the cut (lighting bolt) button is on, then the THC button will be enabled. This is only operative in Plasma cutting mode. With THC depressed, running a program will cause the torch to find the pierce height, start the arc and cut using arc voltage control. When not depressed the unit will find the pierce height but after cutting begins, no automatic height control will be used. Only the jog buttons will change torch height. The THC button turns on the Automatic Height Control based on the Arc Voltage. This compensates the torch height based on feedback from the arc voltage. The THC button can be turned On and OFF pro grammatically by the M-Codes M26 (on) and M28 (off). For changing it during a cycle.

Start Functions

The area below the Jogging Functions on the main screen handles the

Start and G-Code Function Buttons

Open Button

This will bring up the File Dialog for selection of a .tap, .nc or .txt file. These file extensions are defaults; file types may be added or deleted under Setup, Machine Settings, Advanced Settings tab. Do not attempt to open another file type, such as a dxf file here. This section is ONLY for G-Codes. Once selected, the G-Code is loaded into the interpreter, and will show up in the main text box. If there are subroutines, they will be in the Subroutine text area, when the program arrives at a gosub (i.e. M98 P100) function call. If the G-Code file you open does not contain an M30 or M02 (either of which are program end statements) an error will occur.

Edit Button

This will a file edit word processor and allow you to change or modify the file you open.

Start Cycle / Step Buttons

Clicking Run G-Code or the Step button will start the sequence. Step processes one line of code at a time, while Start Cycle will read ahead. Stepping thru a g-code is OK for debugging, but not suggested while plasma cutting

Feed Hold Button

This will stop the plasma torch and ramp the speed to zero on all axes thereby stopping any movement

Resume Button

Resume will restart the plasma torch cycle (go down, search for the plate, find pierce height and initiate arc) and then speed back to the designated feed rate.

Reset Button

Clicking Reset while in a FEEDHOLD condition will stop the current execution and reset the file to the first line again. This is the preferred way to halt program execution. If you would like to stop the program, first select Feed Hold. Once the axes have stopped, you can then click Reset G-Code, which will place the system back in manual mode.

Feed rate and Rapid overrides

On the left box is a selection for rapid traverse feed rate. Default is 100%. You may not exceed this speed but you may reduce it as desired by 10% increments to a minimum of 10% using the up/down buttons. On the right is the override for cutting feed rate. Actual feed rate is determined in the program to be run by the “Fx.xx" G-code command. This multiplier will be used against the program feed rate. Minimum is 5% and maximum is 200%. These feed rates can be changed at anytime. If executed during a move, the new feed rate will take effect momentarily. Rapid overrides will takes effect at the next rapid move.

Dis-connect / Connect

Enables the “simulation mode”, which allows you to run through the G-Code program and watch its movement in the display area. No motors will move during this mode. If your path looks correct, it may be safe to begin with your motors moving by selecting Connect to go back Online.

STOP (Space Bar) (hidden under the jogging buttons when not in a cycle)

Clicking this button or pressing the Space Bar shuts off power to all axes. This is the best method to stop movement quickly. Doing this does not lose the axis position, and re-homing is not required. If a motor has been shut OFF, selecting the check box next to the axis label will restore power to the motor, and servo in position. If a red status-indicator located below the numeric display is on, clicking that area will clear the error indicator. If it returns to ON, the error is still present.