Post Processing for Mach3 (CrossFire)
We cover installing the Mach3 Plasma Post configuration and post processing our
Note: To install Personal Posts on Fusion 360 in MacOS, please
follow the instructions provided by Autodesk.
Post Processing for FireControl (CrossFire PRO)
The following guide provides instructions for generating cutting programs in Autodesk
Fusion 360 for running in FireControl software. This guide assumes that you are
already familiar with performing CAM operations in Fusion 360 for creating cutting
programs; if not, we suggest first watching our Fusion 360 CAM video
series (videos 1-4) in this guide before proceeding.
If your CrossFire machine is equipped with a powered Z-axis, you will want to
go back and make sure that the box for ‘Keep Nozzle Down’ is left unchecked
in the Linking menu of your CAM settings.
When creating your toolpath in Fusion, there is no need to set any values in the
'Heights' tab. Pierce and Cut Height Values will be set in the Post Processing
By this point, you should already have a valid toolpath created in Fusion 360
for your part similar to what is shown below.
Next, we are going to generate a G-Code file for this tool path using the Post
Processor in Fusion 360. A G-Code file is a set of text instructions that are
fed to the CrossFire CNC electronics box through FireControl software for
telling the machine where, how, and when to move in order to cut out the part.
To do this, click on the Post Processor icon (below) in the Additive menu bar.
If this is your first time posting a program for FireControl in Fusion 360,
you will need to open an internet browser and download the ‘Langmuir Systems
Fusion 360 for FireControl Post Processor’ file from the Downloads page on our
website. Once the file downloads to your computer, open up the folder where
this file is stored and right click and copy this file.
For MacOS users, please
follow the instructions provided by Autodesk for installing Personal Posts for Fusion 360.
Go back to Fusion 360 and click the ‘Setup’ button in the Configuration Folder
subheading and select ‘Use Personal Post Library’ as shown below.
Note the file name that now shows up in the Configuration Folder text field.
You will need to navigate to this folder on your computer using the Windows File
Explorer (Use Finder in for MacOS).
Once you have located this file, you can now right click and paste the downloaded
file from Step 5 into this folder. It should look like the folder as shown below.
You can close the folder on your computer after completing this step.
We now need to close and re-open the Post Processor menu in Fusion 360 for the
changes to take effect. Close the Post Processor Menu in Fusion by clicking the
‘X’ in the top right corner of the menu and then re-open it by again clicking
the Post Processor icon (below) in the Additive menu bar.
Repeat Step 5 by clicking the ‘Setup’ button in the Configuration Folder subheading
and then click ‘Use Personal Post Library’. After doing this, you should now see
the CrossFire FireControl Post selected in your Post Processor Menu as shown below.
Next we need to designate an output folder for the g-code programs that we
are going to create. We recommend first creating a folder on your Desktop
that you can store these generated programs in. To select an output folder,
click the square icon with 3 dots next to the text field for Output Folder
and locate your desired output folder for your programs. Here I’ve created a
folder on my Desktop titled ‘Fusion 360 CrossFire Programs’ for easy access.
Next, in the Program Settings subheading we can type in a Program Name or number
and a Program comment (as needed). Then, select the appropriate units for your
cutting program and uncheck the boxes next to ‘Reorder to minimize tool changes’
and ‘Open NC file in editor’. Your Program Settings should look similar to what
is shown below.
Next, we are going to enter our desired cutting parameters for this program.
Below is an explanation of these Properties and how they affect your cutting
program. You can disregard any other properties not mentioned in this menu as
they should be left to the default settings.
- Cut Height (in): This is the desired cutting height for your plasma torch above the surface of the plate. Consult your plasma cutter documentation for the ideal cut height for your torch and material. If you are using a CrossFire without a powered Z-axis, set this value to 0.
- IHS Springback (in): Use this value to add additional cutting height to your plasma torch when cutting on thin gauge sheet metal to account for the force of the IHS switch. The IHS switch applies approximately 2lbs of force to your material when detecting the plate height and this springback value can compensate for the deflection. If you are using a CrossFire without a powered Z-axis, set this value to 0.
- IHS: Use this toggle to enable or disable Initial Height Sensing switch on your machine. If you are using a CrossFire without a powered z-axis, set this value to No.
- Pierce Delay (sec): The pierce delay value is the amount of time that the torch remains stationary after firing in order to fully pierce the material before moving down to the Cut Height. The pierce delay is dependent on your plasma cutter and the thickness of material being cut. Please consult your plasma cutter documentation for appropriate pierce delay settings for your cutter.
- Pierce Height (in): The pierce height is the height above the plate that is used for the initial piercing process. The pierce height should be larger than the Cut Height and is typically about twice the value of the cutting height. If you are using a CrossFire without a powered Z-axis, set this value to 0.
- Retract Height (in): The retract height is the height above the plate that the torch retracts up to after finishing each cutting loop before rapid moving to the next cutting loop. This retraction is key for avoiding tip ups and warped material when moving the torch to the next cutting location on the material. Please make sure that your selected retract height does not exceed the Z-axis travel limits of your machine. If you are using a CrossFire without a powered Z-axis, set this value to 0.
- THC: Use this toggle to enable or disable THC for your cutting program. If you are using a CrossFire without a powered z-axis, set this value to No.
Typical Properties for CrossFire without
Typical Properties for CrossFire with Z-axis and THC
After completing your cutting properties, click the Post button (below) to create your g-code
program. Your program will be stored in the Output Folder from Step 10.
Finally once your program is created successfully, you can now open FireControl
and upload your program for cutting.
Post Processing in SheetCAM for FireControl
The following guide provides instructions for generating cutting programs in SheetCAM
software to run in FireControl by using the Langmuir Systems FireControl Post Processor
file. The FireControl Post Processor will create g-code instructions specific to your
CrossFire machine including IHS sequences, THC activation points, and rapid retract
moves. This guide assumes that you are already familiar with performing CAM operations
in SheetCAM for creating cutting programs; if not, we suggest first consulting the
SheetCAM User Guide before proceeding.
To start, you will need to navigate to the Langmuir Systems Downloads page
and download the FireControl - SheetCAM Post file. After the file has downloaded,
navigate to the Downloads folder on your computer and copy the FireControl-v1.1.scpost
file that you just downloaded.
Next, you will need to navigate to the folder on your computer where the
Post Processor files for SheetCAM are stored so that you can copy the
FireControl-v1.1.scpost file into this folder. On most Windows computers,
the Post Processor folder is located at C:\Program Files (x86)\SheetCam TNG\Posts
but you will need to verify this on your own system. After locating the folder,
paste the copied Post Processor file from Step 1 into this folder. Your folder
should now look like the folder shown below showing the FireControl-V1.1.scpost
Next, open SheetCAM software and click Options > Machine
from the top Menu bar.
Under the Machine Type tab make sure that Jet Cutting is
selected and Rotary Cutting is de-selected as shown below.
Next, under the Post Processor tab make sure that your desired Output file
units, desired Output folder, and Z Zero (should be Top of Work) are configured
correctly. Next, click the drop down bar under Post Processor and select
FireControl-V1.1 like shown below. Finally, click [OK] to exit the menu.
After selecting the FireControl Post Processor, we are now ready to create
programs to cut in FireControl using SheetCAM as normal.
If you are using the CrossFire PRO or a CrossFire machine with a powered
Z-axis, you will need to input settings for Pierce Height, Plunge Rate,
and Cut Height when creating a plasma tool in order to activate the IHS
sequence. For pierce height and cut height, please consult your plasma
cutter manufacturer for the appropriate values.
Note: If you are cutting on thin gauge material, we reccommend adding additional height
to your Cut Height in order to compensate for the material springback during IHS.
For the plunge rate used
for the IHS sequence, we recommend using a rate of 100 IPM. Please also
note that the FireControl post for SheetCAM has a hard-coded 1 inch rapid
retract move after each cut loop is completed by default (after M5 torch OFF).
If you are using a CrossFire machine without a powered Z-axis, be sure to
set both Pierce Height and Cut Height to 0 in order to omit the IHS sequence
from the generated g-code file.
Below is an example of a plasma tool configured for a Razorweld 45A cutter
used on the CrossFire PRO.