How to Create a Toolpath in SheetCam
Sunday, August 30, 2026
You have a finished DXF. Your table will not cut it. It cannot — a DXF is a drawing, and a plasma table needs G-code, which is a list of instructions telling the machine where to go, when to fire, and how fast to travel.
The software that turns one into the other is called CAM, and SheetCam is what most plasma owners end up using. It is inexpensive, it was built specifically for plasma and routers rather than adapted from milling software, and it does not fight you.
Here is the whole path from DXF to a file your table will run.
The four things SheetCam needs to know
Before any of the clicking, understand what you are actually telling it:
- What the part looks like — that is your DXF.
- How big the working area is — that is your job setup.
- What the torch does — amps, cut height, pierce height, pierce delay, feed rate. That is your tool.
- Which side of the line to cut on — inside, outside, or on the line. That is your operation.
Everything in the interface is one of those four things. Once you see that, the software stops being intimidating.
Step 1 - Set up the job
File then Job Options, or it prompts you when you start a new job.
Set your units first — inches or millimetres — and get this right before anything else, because changing it later re-scales everything.
Set the material thickness. This matters more than people expect. SheetCam uses it to work out lead-ins and to warn you about geometry that is too small for the kerf at that thickness.
Set the work area to match your table. Not bigger. If SheetCam knows your table is 4x4, it tells you when a part will not fit instead of letting you find out with the torch.
Step 2 - Import the DXF
File then Import Drawing. Pick the DXF.
Two things to check immediately:
Is it the right size? Use the measure tool on something whose dimension you know. DXF files out of Inkscape very often come in at the wrong scale — this is the single most common problem in the entire workflow. If it is wrong, SheetCam will let you scale the drawing on import.
Did everything come in? Look for missing pieces and stray lines. If your design had a guide circle you forgot to delete, it is in here now and it will get cut.
Step 3 - Create a tool
Tools then Add Tool then Jet Cutting Tool.
The numbers you need come from your torch manufacturer's cut chart, not from the internet and not from me. Every consumable set, at every amperage, on every thickness, has published numbers. Hypertherm ships them in the manual. Everyone else does too. Find yours.
What you are entering:
- Kerf width. How wide the cut is. Usually 0.04 to 0.09 inches. Get this right or your parts come out undersized.
- Feed rate. Inches per minute. Too slow and you get dross on the bottom and a wide, ugly kerf. Too fast and the torch does not cut all the way through.
- Pierce height. How high the torch sits when it starts the pierce. Higher than cut height so the blowback does not destroy your nozzle.
- Pierce delay. How long it waits after firing before it starts moving. Thicker metal needs longer. Too short and the torch starts travelling before it is through, which drags a nasty gouge across the start of the cut.
- Cut height. Where it sits once it is cutting.
Save this tool with a clear name that includes the amperage and the thickness — something like 45A 14ga — because you are going to build a small library of these and in six months you will not remember which was which.
Step 4 - Add the operation
Operations then Inside Offset, Outside Offset, or No Offset.
This is the part that decides whether your parts are the right size, and the rule is simple:
- Outside offset for the outline of a part you are keeping. The torch runs outside the line so the part comes out at the drawn dimension.
- Inside offset for a hole. The torch runs inside the line so the hole comes out at the drawn dimension.
- No offset for scribing or marking, where you are not removing a part.
Get this backwards and every part comes out one full kerf width off. On a small part that is the difference between fitting and not fitting.
Select the contours the operation applies to, pick your tool, and set the lead-in and lead-out. A lead-in is a short entry path so the pierce happens off the part edge rather than on it. Piercing on the line leaves a divot in your finished edge. Use an arc lead-in where there is room; use a short line where there is not.
Step 5 - Look at the simulation
SheetCam draws the toolpath and will animate it. Watch it.
You are looking for:
- Pierces on the part edge instead of on a lead-in.
- Rapid moves crossing over a piece that has already been cut loose. A cut-loose part can tip up, and a torch travelling over it at rapid speed hits it. Reorder the cuts so the outline goes last.
- Doubled paths — the torch cutting the same line twice.
- Anything cut in the wrong order. Interior holes always before the outside contour. Always. If you cut the outline first the part is free and everything after that is a gamble.
Step 6 - Post process
Options then Select Post Processor, and pick the one for your controller. This is not optional and it is not generic — a Langmuir Crossfire wants different G-code than a Mach3 machine or a Fusion controller. SheetCam ships with dozens.
Then File then Save G-code. That file goes on the machine.
The mistakes that cost sheets
Wrong post processor. Runs, looks fine for a second, then does something violent. Check it once and never think about it again.
Wrong scale on import. Costs a whole sheet, every time.
Offset backwards. Parts come out a kerf undersized and you do not notice until you try to assemble.
Pierce delay too short on thick plate. Gouged starts on every cut.
Cut order not set. Small pieces tip up and get struck.
Every one of those is caught by spending thirty seconds looking at the simulation before you save the G-code.
Watch the whole thing
[Watch: How to Create a Toolpath in SheetCam for CNC Plasma Cutting](https://www.youtube.com/watch?v=beLn0SNxG54)
Files that toolpath cleanly
Half the trouble people have in CAM comes from geometry that was never right in the first place — open paths, doubled lines, unbridged islands. Every file in the [Tin Man Metal Works store](https://www.tinmanmetalworks.com/hero-theme-store-front) is drawn for plasma and tested on a real table, and the [free cut file library](https://www.tinmanmetalworks.com/blog/free-cnc-plasma-cut-files) will give you clean files to learn on for nothing.
For the whole chain — design, toolpath, cut, finish, price, sell — the [masterclass](https://www.tinmanmetalworks.com/start-today) runs through it as one process.
The short version
Set units and thickness first. Import and check the scale against a known dimension. Build a tool from your torch manufacturer's cut chart, not from guesswork. Outside offset for parts, inside offset for holes. Lead-ins so you never pierce on the edge. Interior features before the outside contour. Watch the simulation. Then pick the right post processor and save.
Get E-Mail Notifications
Hi, I'm Charles Woten
Owner : Tin Man Metal Works
"Hey there! Thank you for visiting my blog—I hope this article provides some helpful insights and advice you can put to use right away. My goal is to give you the tools and knowledge you need to succeed. If you’d like to stay updated on future posts, feel free to join the mailing list at the bottom of the page.
Thank you again for being here. I want nothing more than to see you succeed and, ultimately, escape the rat race!"
Don't forget to sign up for blog notifications below if you found this article useful.
