When I first created in Fusion 360 the tool corresponding to my Plasma Cutter (Primeweld CUT60) I set the kerf size the same as my IPT-60 torch nozzle that is 1.1mm, without thinking too much about it.
I did not care too much about it so far, but now I’ll have to work on stuff where dimensional precision is more important. What is the best practice, run a straight line cut and measure the kerf with calipers? What do you guys do?
Cut a square on the line (not inside or outside) and the kerf is the size difference between target dimension and actual dimension.
We can thank Perfessor @jamesdhatch for this.
The actual kerf is probably about half that. What the post-processor step is going to do is back off half the kerf amount on inside or outside cuts so the edge of kerf is running on your line and your cut size is spot on. Typically that means you’d end up with the center of the plasma arc running about 0.028" parallel to your line not on the line itself but the edge of the arc would just kiss the cutline.
The value changes by tip, consumable condition, material, power and speed but will generally be roughly in the 0.055-0.06" range. If you want high precision you need to test for the material & settings you’re going to use. But if a couple thou precision is close enough, you can generally get by with using a single measured value.
To do that I just select “in controller” when creating the setup so that the profile will not have kerf compensation?
Everything you said makes a lot of sense, thank you, however:
manoweb> “I set the kerf size [to] 1.1mm”
jamesdhatch> “The actual kerf is probably about half that.”
jamesdhatch> “The value […] will generally be roughly in the 0.055-0.06” range.
But 55thou is 1.39mm, that is … more than the nozzle size, not half of it 
Sorry. I was on the Mars lander mission we don’t do metric well 
You’re right. In mm you’re likely going to want a 1.4mm to 1.5mm kerf setting so you may already be in decent shape. The plasma arc is going to be bigger than your tip orifice - it spreads in a cone the further from the tip you go. That’s why you can’t get perfectly perpendicular cuts in thicker materials. You’ll always get some slope to the sides of the cut, whether that’s within your tolerances is something you need to assess.
Lasers have 1/10 the kerf of the plasma (my laser kerf is 0.007"). But they still have a cone shaped beam, it’s just the slope is less. CNC routing is the only potentially near vertical cutting method (within the limits of the end mill’s flex).
well the nozzle is specified in mm on its side so that’s why I originally used mm.
No I understand what you are saying and I believe some 5 axis water jets can compensate for the conical kerf, but I don’t think I’ll need that 
However, I was curious to know what most people do. The kerf setting is just mentioned in Langmuir’s videos and instructions, and I have found very little in the forum. I will perform some tests and see what I can achieve.
I think most people start with what they see in the Langmuir videos. If it’s important (because they’re making parts vs artwork) they do the cut & measure process so they can dial it in and don’t end up with badly sized parts.
For some part making you don’t even want to try using the plasma - like making bolt holes in your material that are less than say 1/4" (or some say twice the thickness of the material); the work hardening and beveled hole makes precision holes a problem. Using a “peck” where it will mark the spot for the centerpoint of the hole is good enough so once the rest is cut out it’s a simple process to drill the holes manually.
Very interesting. I didn’t realize plasma cuts would work harden the parts.
I like the idea of what you described as a “peck” and I definitely designed parts before with an undersized diameter to be reamed out later. However, I am curious - is there a formal way to design a “peck” in Fusion? Ideally something that has the final size in the design environment but some sort of replacement for small.holes in manufacturing - I’ll have to look it up
Yep. The edges of holes get that. Sometimes makes it harder to later ream or drill out to final size.
There should be. But I haven’t done it. I started using the peck method after I switched to Sheetcam. I would think a similar drill operation could be defined in F360. There are a bunch of posts here about using the technique.
@TomWS is the expert in the technique.
After spending my career watching high priced consultants come in to give us their ‘expert’ advice, I concluded that the definition of ‘expert’ is anyone who traveled more than 50 miles from their office. And, since I am traveling right now, I guess I would qualify. However, since I don’t use conFusion360, I won’t claim any expertise in that domain.
SheetCam is easy. You don’t need to do anything special with your design. SheetCam will use the exact center of the hole if you use a Drill operation. Do a short pierce burst and it will leave a nice centerpunch where you want the hole. As @jamesdhatch said, the details are posted. Useful search term would include ‘small holes’ and ‘peck’.
Well - I am not even close to have enough siderurgical knowledge to be justified to nit-pick but my understanding is that the nitride layer generated by a air plasma cut is not work hardening, but a form of case hardening. Take it easy, I just want to learn the appropriate terminology.
OK but to me Fusion 360 (that happens to be the program I used since well before I entartained the idea to buy my own plasma cutter) is the place where I design fully parametric 3D parts, some are 3D printed, some go through FEA to study the failure points when subject to forces, some are milled and some are flattened, 2D plasma cut, bent and welded. My understanding is that sheetcam is not even close to have all these functions.
SheetCam is only a CAM program so, yeah, it wouldn’t have the functions needed in a full 3D CAD program. I’m not disparaging Fusion360 and it makes sense for those who need those functions. I’m just saying that I don’t use it so can’t advise how to use for peck operations (or anything else for that matter).
Yes understood. I’ll look up how sheetcam implements it and see if an equivalent can be made out in Fusion! Thanks.
Isn’t that the deal where we define a tool with say .249" kerf and then draw a .250" hole where we want the center punch to occur? No lead-in’s/out’s. A short pierce and a real small move for the hole? Put these in their own operation and go to town?
Oh so the abstraction could be performed at the tool level? I’ll look it up and maybe ask on the Fusion360 forum’s about that, it sounds like an advanced technique 