I think I have another example of the problem with cutter compensation. My program isn't the most elegant to begin with so I'd appreciate it if someone would see if it's my problem or Machs.

Load the attached Gcode.
Be sure to set tool 1 in the tool table to have 00.00 compensation so you can see what the basic pass should look like.
Zoom in at the top of the profile and you'll see I have a very small diagonal tool path to get the tool away from the part so the plunge does not leave a mark.
If you run the program you'll see the path is fine and the tool goes off the part, plunges, and comes back in and goes on its way. You can watch it runs this path several times fine going off part on each pass ok.

Stop it, Set the toll offset for tool 1 to say .020. Save. Regenerate the tool path and run again.

This time the tool still goes off the part ok on a diagonal but when it comes around for the second pass it follows a different diagonal to get to the end of the leadin line and exits on the old path (effectively missing milling some of the part). The bigger the tool offset the larger the angle in and out of the diagonal (and the more of the part that's missed).
  If you pan left over to where the tool changes direction from coming up the left side to where it comes across the top, you can see it does that corner on a diagonal instead of square. This chops off the corner of the finished part.

My problem?

Sage

That's good news! I will be eagerly awaiting the update. 

Hi Sage,

do you have CV (G64) set to on, if so that will cut the corners off and change the path, set your finish path to exact stop (G61) and run the code again. This will make Mach stop on corners and produce sharp angles.

Graham

The path is fine sharp corners and all until you apply the compensation. Have a look at the path generated by my code. In the bottom left corner the compensation dissapears all together which sets it up for the next corner to be cut off as described.
I put a G61 in the program and also set "stop CV on angles > 45" in general config and no difference.

Sage

Hi Sage,

Looking at your code I think it is at fault.

Post a sketch of your part along with the dimensions and I will code you a program and lets see if it works, what cutter size are you using.

Graham

Graham:

The best I can do is give you a DXF of the original drawing (attached). But it's been through a lot to get where it is (posted previously)
The process I followed (with great pain) is as follows:

I used LazyCam to create an outside offset so I could cut the profile with a 1/8 cutter.
I used LazyCam parameters to make it take multiple .020 passes. To .380 depth,
That's basically what you see if you don't add any cutter compensation to what I posted.

After each pass it stops and plunges another 20thou but that left a divot on the side of the finished part so I manually added the little 45 angle to the side to get away from the part a bit to plunge and then return.
It had to be run pretty slowly otherwise the cutter would get in trouble when cutting at depth (.380).
I decided I could speed it up if I used a 1/8 hogging mill to get most of the metal out and then use a standard mill to do the finish cut.
Rather than go back to LazyCam and create another offset for the rough cut I figured I would just use the cutter compensation to make the rough passes and call the subroutine again without the compensation to do the finish pass(es).

Having said all of that I hope you understand what I'm doing. I have no doubt that you can write a whole new program.

BUT

I have to ask. The program I posted is pretty simple and it works fine without the compensation. Rather than spend your valuable time creating something that is completely different. It may be more beneficial to the understanding of the problem to figure out what's wrong with my program. There must be some aspect of it that Mach does not like and it might point to a problem that needs to be fixed in Mach (or not). Or that will help me understand the programming pitfalls.

Suit youself, you know a lot more about this than I do.

Thanks


BTW this is only a simplified version of the real part I need. Reduced to the simplest version that exhibits the problem.
Sage

You're not allowing enough room for the comp to be applied. You need to start at least the tool radius away from the part. Here's how I do it.

ger21:

Thanks for that. It's pretty cool. I'll have to analyze it though because I see that you have drawn "horns" on the corner of the part but they aren't even used in the resulting tool path. So I'm a bit confused how the tool path was created unless the compensation function created it's own path based on whatever it saw fit. Then I have to ask why did you make the "horns" with 45's on them when straight lines out from the corner - your suggested two cutter diameters or so  - would have sufficed.

I get your point though about the lead in/out needs to be bigger. My little attempt at that was an after thought just to stop the divot that was giving me trouble. I didn't know it was going to be a problem with the tool offset - also an after thought.
You'll notice that my little lead out is a relative move away from the part and I expected it to always be the proper amount since it was relative. I guess it was just to small.

Let me look it over and analyze what going on bit more.

Thanks

Sage.
 

At the start of the line, the center of the tool is on the vertex of the first line. Comp is applied while moving to the second vertex. At the second vertex, the tool is tangent to the first line and second line. I usually just extend the line by the tool diameter, which ensures that comp is applied outside the part. I also ramp in during the lead in, so I'll usually make the lead in even longer, to give a shallower ramp.

One other thing. You don't actually need the leadout move I used. The machine I use at work requires it, but Mach does not. Just make sure you move at least the tool radius, maybe more, beyond the part before calling G40. You can also lift the tool before G40, just to be safe. This is the same code without the leadout.