Started cutting today and was able to do a few trials that turned out near perfect. Now my question is this:
on hole diameter, I command 0.2" in the design and I get 0.182. On the part width I command 2.811 and I get 2.841.
Is adjusting the kerf diameter where I should tight up those tolerances? It seems to make sense to me, if I command X amount of kerf in the setting, but it is less in actual (what the machine actually removes) then it would make sense why the both are happening. (Holes being cut using inside line, while the outside of the part is cut on the outside line).
In addition, is there a minimum limit on the torch piercing delay? How fast can we go in the software?
I’ve noticed the same on my holes but I just account for it in fusion when making the program. So my 1/4” holes are .270 instead of .250, 1/2” holes are .520 3/4 is .770 etc… not really a big deal to me but that’s what I do to fix the issue
There’s always a bit of run out or variability with Plasma cut holes. If you have a hole that must be X. The best way is to under cut it on the plasma. Then drill and ream to size.
right, do a pilot hole and thnn ream to whatever size it must be. I was just curious if my logic was sound when it came to adjusting kerf size to get to the closest possible machine tolerance…it’s an ocd thing for me and just a need to know/understand
All plasma cut edges will have some bevel, typically around 3 to 5 degrees. This is especially true for holes. When i am cutting bolt holes, I always draw the hole larger (same as what @oneupperformance described). Over time you will get a feel for how much larger you need to make the holes in order to have the bolts go in.
Now if I am doing a part that has critical hole size requirements, I will cut the holes on the plasma significantly smaller than the final size. The reason is because the plasma cutting process creates a very hard nitrided layer that is about .015" thick. If you try to shave off .010-.020 with a reamer or a drill, you are likely to trash it very quickly. Now, if you plasma cut the hole .100" or so undersized, the cutting edges of your drill will be able to get under the hardened surface.
One other tip, always drill from the back side of the part as it will further prolong drill life.
@mirage2991
Might try to decrease kerf diameter by .020-.030 in tool setup assuming cut quality, feed rate and amperage are all good.
If you find that one number doesn’t work for both inside and outside cuts then I might try to setup 2 different “tools”. One for inside cuts and one for outside cuts. Inside tool kerf -.018 and outside tool kerf +.030 of what kerf is currently set at.
As far as pierce delay. I would keep reducing the delay until you find what works for you. Guessing you are cutting thin material and pierce delay is set to 2 seconds.
pierce delay is at 0.25 sec right now on 14gauge metal…I was messing around with 24gauge earlier, that worked well as long as the brought the machine down to 15A . Thanks for the idea on the kerf settings…haven’t messed with it.
Not to be “that guy” but cobalt drills are HSS it’s just a blend that has cobalt (5-7%) in it. But it is the better choice for flame/plasma cut holes. Don’t go at them with a carbide bit. Carbide will cut really hard stuff but it’s super brittle using it in a screw gun on a rough hole has a high likely hood of chowdering up the cutting edge in a hurry!
Agreed, I should’ve mentioned M35 HSS, and not the coated stuff either but the real deal.
Yeah, definitely would not suggest a cobalt mill bit, could very well end up having it chip off into your face or just mar up the work piece. Right tool for the right job, right? Lol.
and just a need to know/understand