We have a new 1100M mill and having problems with using G41/G42 cutter compensation. Initially we were getting the error “line entry move length is not greater than the tool radius”. Got past that by adjusting the lead in to a move larger than the tool radius (annoying but ok…). But my problem is regardless of where I put the G41 or G42 in the code, it is being ignored. Still cuts “on the line” with no tool offset. I’m attempting to cut a hex to a specific size (.371 A/F) with a .312 cutter and the part always comes out about .060 A/F. I did put a ticket in. Just curious if anyone else has experienced anything like this. I noticed all the example projects don’t use cutter compensation. How is that possible to get a specific size without adjusting the code to allow for a specific tool size?
Are you hand-coding, using CAM or conversational or what? The tool diameters are set or are you using the D-word?
I use cutter comp for wear with CAM, but don’t mess with it by hand.
This particular case was hand coded. I don’t currently have access to the code at the moment. ‘But we’ve tried moving the G41 to various lines around the first G1 line and last G0 line. I’m saying we-because I am not the only person involved. It plots correctly on the screen, but does not show a tool offset and cuts what it shows on the screen.
I’ve tried both G41 and G42 with the same results. The current code shows G41 and is cutting clockwise around the part.
You aren’t using tool zero?
Is the diameter set in the offsets table or are you using the D- word with the G41?
I’m kinda in the same boat. Don’t normally program by hand. But this is our first Tormach and it was a simple program that someone else wrote. I attempted to add the cutter compensation. I posted out for a different machine and it looked similar - so it should work.
Tool is not set to zero in the tool offset table. Tried it both ways - with and without the “D” word. No change.
We are having other random problems with the machine too. I think something is corrupt in the PathPilot software. Can’t generate an engraving program at all using the fonts supplied in the machine.
Tool #0 is also doesn’t comp AFAIK. Probably not it if you have other things going on.
As far as I can tell, it is set for tool 3 and tool 3 is showing on PP when running the program. The tool dia. is set to .3125 on the offsets page. Unless I’m missing something in the tool call in the program to make it read the tool dia. …
Started my work computer…
Here is the code we are trying to run…
(0.371 HEX)
G90 G54 G64 G50 G17 G40 G80 G94 G49
G20 (INCH)
N10 (2D CONTOUR)
T3 H3 M6
S3350 M3 M8
G54
G00 X-1.5 Y-.5
G43 Z1.
G00 Z.5
G01 Z-.2 F5.
G41 G01 Y-.20404 Z-.2
G01 X0.0 Y.39462
G01 X.34175 Y.19731
G01 Y-.19731
G01 X0.0 Y-.39462
G01 X-.34175 Y-.19731
G01 Y1.0
G40
G00 Z2.0
M30
What version of PP are you running? There was a bug with engraving that got fixed recently which makes me wonder if you are up to date.
Cutter compensation works from CAM each time I’ve used it but I didn’t go to deep into the details of where everything fits
It is V2.12.3
I’m aware it is up to V2.13.0. Will need to update to that.
The other thing that I noticed was the hex on the part was incomplete. The first flat was not cutting.
G41 G01 Y-.20404 Z-.2
G01 X0.0 Y.39462
the Z-.2 above was added to make sure the tool was at the proper depth (repeat of the previous Z-.2) When single stepping, it showed no change in distance to go but would not cut on the first flat.
The G41 (or G42) line needs a D-word to tell the control which cutter offset to use.
i.e. G41 G1 Y-.20404 D3
It works better to approach the path roughly perpendicular to the path using an approach at least longer than the radius of the tool. The program is approaching it from the wrong side of the path as well. (Y-.5 to Y-.20404) If the rapid prepositioning move was to X-1.5 Y.5 then the G41 move to the existing Y-.20404 (with D3) I think it might run.
Art
George,
You also need to add the G43 call for the offset, as written the machine should crash.
Thank you,
Norman
I did try it both with and without the D word with no change (yes, T3 has 0.3125 dia.). According to the manual, without the D word, it is supposed to assume the current tool. I am well aware of ass-u-me ing but did not see a difference.
I kinda came to the same conclusion about the roughly perpendicular approach but didn’t think about it when I was at the machine. I was asked to troubleshoot the problem but didn’t write the original program. I usually program using CAM software not by hand.
I discovered the PP Hub this weekend. When I put the program into it, I noticed the line it plots is ALWAYS the center of the tool. When you add G41/G42, it adjusts the line shown by the offset. I was assuming the line was the programmed path and the tool would be offset when adding G41/G42. I was wrong. That might be a better way to visualize that you are using the correct offset though. The current way doesn’t necessarily let you know you are getting the desired part.
G43 is in the program.
G00 X-1.5 Y-.5
G43 Z1.
G00 Z.5
but probably should be G43 H3 . Does it require a move like G41/G42 to enable? Or is it fine on a line by itself?
The code looks a lot like what Fusion 360 outputs and seems unlikely to have been written by hand with five decimal places, so is it possible to go back to the source and re-post with a recent Tormach post just to see if it does anything different?
Hi George!
I had never been to PP Hub, awesome! Tried running your code with T3 = .3125 and it runs but cuts way oversize. The geometry in the code already has the .156 tool radius added to the .371 hex. So to get on size you would use a tool offset of T3= 0. (The wear offset method) To start slightly oversize, use a diameter of .005 or .010. Measure the result and reduce as needed. If your tool is smaller than nominal, use a negative size for the diameter (T3 =-.005). You can ease into the correct size by simply re-running the code after the tool offset update. A great help versus changing your CAD or CAM and reposting to “fix” it.
Your code seems to work as written with the G43 called at the first Z move and no D word with the G41 (seems to default to active tool). Even starting from the “wrong” side wasn’t a problem.
I see what you are saying about the display- it draws the center line path of the tool, but if you note the grid scale or the coordinates the path is drawn larger with a larger tool .
This “wear method” is especially helpful if you want to use G41/G42 inside a feature that isn’t much bigger than the cutter- instead of needing an approach that is half the tool diameter, it only has to be half the wear amount.
Hope this helps!
Art
Roy,
I can guarantee it didn’t come from Fusion 360. It was definitely hand written but not by me.
Art,
Yes I noticed the scaling change too. I still think it would be better to show what is programmed and show the tool to the side of the line if using tool comp. - just my .02 on that - but at least I’m aware of how that works now. But when we cut the actual part, it was coming out way small - like about .090 A/F regardless of changes in offset … and the first line wasn’t cutting with no change in Z and it showed correctly on the screen. It’s a brand new machine so l put a ticket in - other things aren’t working as expected too. Conversational engraving only gives “Hello World” regardless of the text posted.