I have tried adding small text ( a website link) to my drawing both in SVG format and text format through Fusion360. Everytime I do my setup and then simulate my cut it skips over all the small text. I have checked the text, no broken lines, tried multiple text types, even the simple one in Fusion. The text is 1/2" tall and shows as being extruded, Larger text right above it simulates the cut fine… what am I missing?
Just curious . What are your lead in and out set to ?
Lead In & Outs set to zero like in Langmuir video shows in their videos.
Did all setups same as in videos:
- 3: CREATING A SETUP
- 4: PROFILE TOOLPATH GENERATION
- 5: POST PROCESSING
I cut some 3/4 letters . Set to 0 like you said and radius to 20 degree .
I am having zero luck with this software. Have it on 2 different PC’s. Working on the same project, software does 2 completely different things on each PC. Also seems like every time I open/use the software things operate slightly different. Yesterday I was trying to extrude a SVG file and it would not let me extrude the file, today it let me extrude it???
I have used a lot of software in my life and this is definately different to say the least. My son is a graphic designer I had him mess around with it and he also said it is weird and it seems like it is controlling what you want to do with it… I am not a fan…
1/2 letters are really small if one tiny area within it is to small it will reject it. And I agree on the program being a real pain , jamesdhatch will jump in and explain it in detail I hope. Don’t give up .
I won’t I have product to make. Would just like to have my logo and website URL on it…
None of your letters are touching each other are they? Ran into a font where capitol r k y waned to touch so I trimmed the corners some to make them cut.
Ima total noob at this. Just running my past hang ups by ya.
Noobie to Plasma here also. Have my table ready to go, been recreating my prints in Fusion and have been messing with this software for almost 3 weeks now… most of that working on this problem…
Sorry none of my past issues helped yours. But there are some very talented people here that will help. Jamesdhatch teaches a lot of this stuff. And some here have been into Cnc for a long time.
Are parts of your letters narrower than you designated kerf width?If you tell fusion your machine will cut a .060 kerf but your drawing has details that are narrower it will not work i dont believe.
1 Like
Would you mind posting a picture of what’s going on? Might help some of us see what might be happening
Yes, this is what it seems like is happening. Larger text works fine.
1 Like
I had the same problem where the spaces between the bottoms of letters wouldnt get cut out because of this so i would go in and trim the letter back till the space exceeded my kerf width then fusion would generate a tool path to that area.
That’s what is was… just ran a simulation & it worked… Thank you Lord Baby Jesus…!!!
1 Like
But you guys already solved it.
Coming from a world where if you can see it in the screen then you can put it on a piece of paper to one where things like kerf and lead-in matter is hard.
At least with a CNC router it’s easier to see that the 1/4" diameter cutter just isn’t going to do the detail because you can see the thickness of the tool. When it’s a beam if light (or plasma) it’s hard to wrap your head around it.
It helps if you’ve ever done scrollsaw work because you learn to “see” the path the blade will take. That’s what you need to do here (the simulation will show it - if you were successful).
It isn’t easy - I can take a plasma or router design and know it will work with the laser - the kerf is only .007" wide. The reverse isn’t true though and I find I have to rethink how much space I have between things and how much room there is inside objects. And be careful when zooming way in because it looks like there is plenty if room until you realize there’s tons of room when zoomed in 800% that disappears on the table
1 Like
So is it possible to set your Kerf to something like .005"? Could you go to 0? I have mine set on .005 right now and it is cutting just about everything I need in the simulator. But what about real life on the table? Will it do this with the tips that came with the crossfire and the Vipercut 30i ?
You can set the kerf to anything you want but you’re not going to change the actual kerf.
Plasma kerf is commonly in the .05 to .07" range depending on power & tip. (And a bunch of other factors but this is close enough.)
What the CAM software is doing when you tell it your torch has X for kerf, then it offsets the toolpath so the outer edge of the kerf is on the line you’re trying to cut. As long as what you tell the software is the kerf matches what the kerf really is, your part will be nearly exactly the size you design in your CAD software - a 2" circle will be 2".
So if your kerf is .06" (and you want the piece of circular metal as the part) then the CAM software tells the CNC to actually move the head 2"+.03" (it uses 1/2 the kerf because that makes the outside of the cut on the 2" line and the other side of the cut .06" away). When it’s done, your piece of metal will be 2" and not 1.94" which is what it would be if it cut right on the line.
Not particularly concerning for art pieces but pretty critical for machine parts you’re trying to make.
So, if you tell the machine that your .06" kerf is .02" your offset will be calculated incorrectly and your part will cut out a little smaller than you drew.
If you tell it you have a 0" kerf, then the compensation will drop the torch tip right on the line.
Since a lot of times the problem with cutting small parts is that the kerf or lead-in values won’t allow the machine to create a path where you can maintain the needed distance to make the part exactly, telling it that you have a 0" kerf will let the toolpath calculate.
But, one of the other reasons you want the machine to calculate the offset is to prevent divots in your part cuts - when you pierce the material it makes a hole slightly larger than the kerf made when the torch is moving so you get a point where the cut is larger than the rest of the line. By specifying the true kerf of the machine and setting sufficient lead-in values you can keep that divot outside the final cut line and the part won’t have any extra tiny holes in it.
I’ve searched the forum for an answer and this thread is as close as I can get, but I’m still having similar issues. The kerf width on my plasma is set to 1.5mm and the letters I’m cutting are roughly 27mm tall with each leg of the letters being between 3.1mm and 4.2mm wide.
I’ve selected the desired profiles and generated the tool path, but SOME of the letters have been missed? As an example, a letter ‘S’ with thinnest width of 4.0mm has been missed, while the number ‘4’ has a thinnest width of 3.1mm has been picked up?
I didn’t explode the test as it still cut everything out using the ‘extrude’ function.
I’m a little lost?