Navigating CNC for Beginners - Seeking Guidance and Clarity

CrossFire ® PRO General Discussion
1

Hey everyone,

I’ve got a friend in his 80s who’s eager to dive into CNC machining with his Crossfire Pro, but he’s a bit lost with all the technicalities. I am not going to be using the machine, but I took on the task of getting up to speed so that I can help him understand and get him going on a few projects.

Hardware Questions: Know Your Machine

  1. Identifying the Model:
  • How can I determine the exact model of the Crossfire Pro I’m dealing with? Is there more to it than just the name?

  1. Understanding the Setup:
  • How do I figure out what head is installed on the machine?

  1. Finding Head Information:
  • How can I accurately determine the specifications of the head being used?

  1. Height Cutting Capability:
  • Does the Crossfire Pro support height cutting (Z-axis), or is it limited to XY movement?
  • We are probably interested in cutting only sheets of metal in 2d, but the height of the metal matters I would imagine.



Software Setup Confusion: Tackling Fusion and Fire Control

  1. Fusion 360 vs SheetCam vs. Fire Control:
  • What’s the distinction between Fusion 360 and SheetCam concerning the Crossfire Pro?

  1. File Types Overview:
  • What are all the file types relevant to CNC, like G-code, Tap files, and DFX? I need a quick grasp of their purposes.

  1. Tool vs. Machine Setup: Most important question most likely
  • What’s the difference between setting up a tool and choosing a machine in Fusion 360? It’s a bit murky for me.
  • Do I need both? Is one default in the Fusion 360 or do I also need to create a machine?
  • Is there a premade file for the machine that I can download - yes I saw the download page but I am not sure what those files are or where to even use them and if I even need to.

  1. Simplifying for the Elderly User:
  • Will utilizing FireShare streamline the process for my elderly friend who might not be so tech-savvy?

Conclusion: Seeking Clarity in the Chaos

I’m on a mission to arm my elderly friend with the knowledge to start working with his Crossfire Pro, but there’s still a lot I don’t know that I don’t know. Any help in shedding light on these questions would be greatly appreciated! Thank you forum!

2

Ok, a lot of information to pass here. Let’s go…

Hardware -

  1. Crossfire Pro - To the best of my understanding, the Crossfire Pro is a 4 x 3 dual gantry system. There is only one version of the table.

  2. The head - Are you referring to the Plasma torch? If so, there are a number of possibilities, depending on the Plasma Cutter one has. Typically, the only two options are hand torch or machine torch. (Hand torch has a trigger. Machine torch is (usually) a long cylinder.)

  3. Head (plasma) specifications - The manual for the plasma cutter will usually offer guidance in this area. Important items to know - capacity, ie what amperage will the cutter go to. From this, and what settings the cutter is set to, we can offer suggestions on cut speed etc.

  4. Height - Yes, the Pro does comes with IHS (Initial Height Sensing) and THC (Torch Height Control) is listed as an option. For most cutting, IHS will suffice. I prefer THC with IHS for my cuts, especially with thinner material.

Software -

  1. Fusion vs SheetCam - Both pieces of software will generate usable G-code (cut files) for the CrossFire Pro. Fusion also has the ability to create the files, where as SheetCam requires the part / pattern to be generated in another piece of software. (There are numerous possibilities here. Some like Inkscape to generate dxf or svg files. I prefer AutoCAD.)

File Types - I’ll break it into G-Code and Design files. G-Code, the files that FireControl can run, are usually .nc or .tap files, processed by either Fusion or SheetCam, with the Langmuir Post Processor installed. These are the files that are loaded into FireControl. DXF (and / or SVG) files are designs that have not been processed. They will require Fusion or SheetCam to convert (process) them into usable G-code.

Tool vs Machine - In Fusion, Tool setup is the important one. (As a mater of fact, I run without a machine setup.) Important settings are cutting speed, kerf width, and lead in / out values. Other items, such as cutting height, pierce height, and pierce delay will be entered during the post process.

Simplifying - FireShare “may” make the process simpler, however I see a number of posts where people download a FireShare item and expect it to cut without issue. I would try to understand what / how the process works, then approach FireShare. If something doesn’t work right, you / they are better prepared to identify and fix the issues.

2 Likes
3

Sounds like a bot asking those questions.

4 Likes
4

Agreed. No one on this forum refers to:

  1. Specifications of the Head
  2. Height cutting ‘capability’
  3. How to determine the exact model of Crossfire Pro

We will see how Michael Bruce responds. And Michael, if you are a real individual, my apologies. We are just having a raft of strange questions from new users. Your questions are worded as if you know something but not enough to ask the right questions.

3 Likes
5

Hi there. Not a bot. I do not know what I do not know. I just wanted to get to the point and its not my machine. Just helping an old timer.

6

Good to know. So back to your issue. Was @Simsworx lengthy response helpful? Do you have more questions. I promise to be polite.

1 Like
7

Thank you very much for the reply. This was all helpful. I got some experience with the cnc today. I created two end caps for pipes at different angles, which required a circle as well as an ellipse. What I noticed is that the head is too high. So too many sparks. We got the speed, power and air pressure correct.

New questions.

  • what is the easiest program to create simple 2d cuts? Fusion 360 is really advanced and has way too many options. I can handle it, but the old timer, maybe not, however, it IS free (for less than 10 enabled projects).

  • When I create a sketch, it is 2d. Since I am working with metal that might be 0.125 in thick (or more), should i extrude the 2d so that the head has awareness? Or do I set the offsets in the setup and only use the 2d simple shapes (not 3d)??

image
image1920×1243 130 KB

I see for stock offset, side offset is very useful. My question is about the top offset, is this where I would set the height of the metal? This has to do with the previous question and understanding where the offsets are vs creating an extrusion in the model itself.

image
image1158×1222 65.9 KB

  • considering the default cut speed was not used today, we did around 69 (used a manual and measurments). Also, the plasma cutter is handheld and the machine that drives the amps is all manual, so do the settings really matter on this screen? We have to dial in the air pressure, and the amps. So it seems that this will always be manual and the cut speed and height clearence is most important to get right in the software.

Am I on the right track? (ill ask a summary of the questions again)

  • simplest 2d software for making simple designs
  • understanding clearence, extrude, and setting offsets, how do I zero this out? Also, can this be edited after gcode creation?
  • tool creation, do those settings really matter? It seems that when the 2d path is created, you need to select a speed and at that point, it could be set.
    — pierce and cutheight?
    — process inputs?

Bonus questions:
Does this Crossfire Pro (along with this handheld IPT-60) do any etching? Or is this strictly for cutting?

Thanks again yall!

8

Wow! You really are convincing as a human! :rofl:

This is a mixed answer and you asked it correctly. If you would have said “What is the simplest program to design a 2D object” there are a myriad of choices. Let’s stay with that thought…
You can design in any program that can eventually generate a dxf or svg file. They are both vector graphics files. There are too many to list but many people use Inscape (free) or Solid Edge or FreeCAD.

Other members will chime in with their preferences. As you might imagine, we are all jaded by what we learned first or became confident with. Everyone has different learning styles but most all of us have used something like YouTube to help refine our knowledge and skill with these programs. There are online courses and people who will help to tutor.

Back to your question: “easiest program to create simple 2d cuts?”. Once you get the vector graphic file, it has to be turned into machine language: These are CAM programs. They are a set of commands that the CNC table is looking for: move the torch and turn it on and off, basically. There are only two choices for this conversion at this time: SheetCAM and Fusion 360. SheetCAM will cost (one-time cost) and Fusion 360 is free. I love Fusion 360 but it took a lot of diligent learning. I would probably steer you to the one-time charge of SheetCAM. Once your tools are set up in SheetCAM and you get the process down, it is pretty slick in SheetCAM.

SheetCAM and Fusion 360 generally only cares about the actual drawing. The way you enforce the thickness and type of metal is thru the “tools” that you set up in either/both CAM software programs. Generally speaking the tools react to the different thickness of metal by the speed of the cut. The amperage and air pressure is set at the plasma cutter and has nothing to do with the CAM process.

As for the cut height: your system sounds like either the gcode (results from the CAM program) is telling the torch to be too high or the IHS (initial height sensing) is not working correctly.

Clearance: you can ignore it right now especially if you are just cutting one item
Extrude: if you use SheetCAM, it is not necessary. If you use Fusion 360, it makes the CAM (manufacturing) process so much easier.
Offset: usually this is set to “left” offset. The plasma stream does the best cut on the right side of the path so you want to be on the left side of the line.
How do I zero this out?: I don’t understand this one. If you want “no offset” you would pick “center” compensation.
Can gcode by edited: Yes if you understand all of the gcode values you could. It is usually easier just to re-CAM it. But, in FireControl you can modify some things after the fact. You can re-scale the image, you can increase/decrease the speed of the cut and you can change the pierce delay without reCAMing the gcode.

The only values that flow thru from the tools is

FusionToolsSettings2
FusionToolsSettings2779×669 43.2 KB

(Now in SheetCAM, the tools values will flow thru once they are set up in SheetCAM). In Fusion 360, you will be taken to another screen during the manufacturing process that basically asks these questions again. They should have looked at your “tool” but they ignored it for some reason:

This is the final screen with Fusion 360 during the Post-processing that you need to enter some of those values that it ignored in your “tool.”

PostProcessing2
PostProcessing21360×858 99.5 KB

Pierce height is where the torch goes to start the cut. It is usually about 2.5x higher than the cut height.
Pierce delay is the delay from when the signal is sent to turn on the torch and the torch begins its plunge from pierce height to cut height.

I have the Hypertherm 45XP which actually has an etching mode. If your plasma cutter and torch can be set to etch then you could etch with the CNC process. It won’t look as slick as laser, though.

9

This is about the torch height issue. You might look at this posting on another topic.

And to clear up some questions with gcode: SheetCAM generates a xxx.tap file and Fusion 360 generates a xxx.nc file. They are basically the same thing to FireControl.

If you would like a brief start on understanding the gcode (I know you said you have some experience with it, so I will give you the nearly complete listing of gcode commands):
G-Code Cheat Sheet of Common Commands.pdf (186.4 KB)
G-Codes Explained_ An Introduction to Common G-Code Codes.pdf (201.6 KB)

I get lost in this one:
Every G Code for Your CNC [The Complete List] - Machinist Guides.pdf (1.6 MB) (some do not apply to plasma cutting)

Here are the most important/often used g-code commands:
G-code explanations with information compiled from notations from @DS690, Langmuir
document (G-Code Command Sheet) and www.thomasnet.com.
This is how the gcode will look at the beginning of each cut loop:
G92 Z0. - Set Z axis zero at the current location
G38.2 Z-5.0 F100.0 - Drive the Z axis down (up to 5 inches) @ 100 inches/min until it opens the
IHS switch on the Z axis
G38.4 Z0.5 F20.0 - Raise the Z axis (up to .5") @ 20 inches/min until it closes the IHS switch
G92 Z0.0 - Set the Z axis zero at the current location
G0 Z0.02 (IHS Backlash) - Raise the Z-axis .02" to account for backlash
G92 Z0.0 - Set the Z axis zero at the current location
G0 Z0.15 (Pierce Height) - Raise the Z axis to pierce height
M3 - Torch on
G4 P1 - Pause (in this case 1.0 seconds for Pierce Delay)
G1 Z0.06 F70.0 (Cut Height) - Lower the Z axis to cut height @ 70 inches/min
H1 - turn on the Torch Height Controller
Additional commands you might see include:
G00 Fast move
G01 Linear interpolation
G02 Circular interpolation CW
G03 Circular interpolation CCW
G17 XY plane designate
G20 Set English units (inches)
G21 Set metric units (mm)
H0 - turn off THC
M5 -torch off

Langmuir adds:
H0 is written into the preamble of every program to ensure that the machine controller has
control of the Z-Axis to perform the IHS sequence:
(v1.6-af)
G90 G94
G17
G20
H0
H1 is written once the torch has fired, delayed, and moved to Cut Height - before starting a cut
loop. Once the cut loop has finished and the torch must retract for the rapid to the next cu, the
Machine controller needs to be in control of the Z-Axis so an H0 is again written, generally
before the Torch Off (M5) command.
And the last line of code must be: M30 - end program
The very last line needs to be the program speed (cut speed) in parenthesis like (PS120) so this
will appear as:
M30
(PS120)
Pre-amble
Version Comment
The first line in a FireControl Posted Program contains a comment that identifies the version
of the post processor that generated the program. This comment is intended for use with the
two Langmuir Systems supported Posts: Autodesk Fusion and SheetCAM.
Note: If you are developing your own post, be sure to use either (v1.6-af) or (v1.6-sc) in the Wrst
line of your program to ensure that FireControl will accept it. If you publish your post online,
please make Langmuir Systems aware by contacting our support team and we can assign a
character code for your post so that future versions of FireControl will accept it without
needing to mask as Fusion or SheetCAM.
Ex.
(v1.6-af)
G90 G94
G17
G20
H0

1 Like