[Mooser]

Somedays it just doesn't pay to get out of bed...

I've been doing some work on my probe here and needed to cut out a simple shape on a circuit board
Basically a circle with a notched out area between 10 and 2 o-clock

I did it up in mastercam x, generated the code and then watched as mach3 did weird and wonderful things to my simple profile

After fighting with this for the longest time, trying to get it to understand, I just broke the code into several section and ran it but I couldn't get over it's inability to understand this shape

By the looks of it, the post is getting the start and end points correct and then connecting them with the proper size rad but doesn't understand that the rad should go outside of the points (it's putting the short part of the rad instead of the long part.

Attached are some screen shots of what mastercam and mach3 see as the same shape.

Any Ideas as to how to handle this other than generating separate paths for everything???
Thanks
Moose
(I'm gonna through this into mastercam and maybe mach forums too)

[pzzamakr1980]

If you are using the Boss post, make sure you delete the line at the beginning, line 3 or 4 where it directs the machine to go to x10y10z10. That will cause problems. Other than that, I use the Boss post with very little modifications. Generally I have to insert G49s to negate tool offsets and add the number after the H to pick the proper tool.

[philbur]

What does the code in Mach3 look like.

Phil

Somedays it just doesn't pay to get out of bed...

I've been doing some work on my probe here and needed to cut out a simple shape on a circuit board
Basically a circle with a notched out area between 10 and 2 o-clock

I did it up in mastercam x, generated the code and then watched as mach3 did weird and wonderful things to my simple profile

After fighting with this for the longest time, trying to get it to understand, I just broke the code into several section and ran it but I couldn't get over it's inability to understand this shape

By the looks of it, the post is getting the start and end points correct and then connecting them with the proper size rad but doesn't understand that the rad should go outside of the points (it's putting the short part of the rad instead of the long part.

Attached are some screen shots of what mastercam and mach3 see as the same shape.

Any Ideas as to how to handle this other than generating separate paths for everything???
Thanks
Moose
(I'm gonna through this into mastercam and maybe mach forums too)

[Mooser]

I'm using the post from the Tormach site, is there a better one out there?

The guts of the Mach3 Gcode looks like this

N220 Z.1
N230 G1 Z-.1 F6.16
N240 G3 X.4688 Y0. R.4687
N250 X.2345 Y.4059 R.4688
N260 G1 X.2343 Y.406
N270 G3 X.193 Y.3968 R.0313
N280 X-.193 R.4412
N290 X-.2343 Y.406 R.0313
N300 G1 X-.2344 Y.4059
N310 Z0.

The comment was made to change the R.4687 to -.4687 (arcs over 180 need negative) which does correct the problem.
I made some changes in mastercam on hte control entry and it generated new code

N230 G1 Z-.1 F6.16
N240 G3 X.4688 Y0. R-.4687
N250 X.2345 Y.4059 R.4688
N260 G1 X.2343 Y.406
N270 G3 X.193 Y.3968 R.0313
N280 X-.193 R.4412
N290 X-.2343 Y.406 R.0313
N300 G1 X-.2344 Y.4059
N320 Z0.

which, although not negative, also seems to work fine, I've got to plot and see if it made the arcs less than 180 deg or what actually happens here.
Mooser

[Freddy Bastard]

Mooser,

You should use the last post I did on the yahoo group. The file name is MPMASTER_Tormach.zip (you need to put .MMD and .control files in C:\mcamx\cnc_machines and put the .pst file in C:\mcamx\mill\posts)

I use it every day, and work's very good. If you have the rotary table, you can use it too. If you've any changes to do I can make it. If you have questions, feel free to ask.

Hope it help.

[keithorr]

The guts of the Mach3 Gcode looks like this

The guts don't count without context. The beginning of the file sets up the environment and expectations. Without seeing all the G00 G17 G20 G40 G49 G54 G80 etc at the top of the file we can't see if the information is being interpreted appropriately.

What are your mach settings? Are you using PCNC3 or Mach3?

You can post the entire file in text or zip and have a better chance at getting an accurate assessment

[Mooser]

I'm using the pcnc version of mach3.

If the two initialization routines were in anyway different I would have posted them but anyway, heres' are two different G-codes from the same mastercam file. one correct and one not.

The profile_fanuc works properly, the profile-pcnc is the problem one.
By changing the config to allow mastercam to break at 180deg on arcs (like it does with the fanuc post) seems to correct the issue, and avoids the "larger than 180 deg need a negative radius" bit.

Mooser

[Mooser]

Mooser,

You should use the last post I did on the yahoo group. The file name is MPMASTER_Tormach.zip (you need to put .MMD and .control files in C:mcamxcnc_machines and put the .pst file in C:mcamxmillposts)

I use it every day, and work's very good. If you have the rotary table, you can use it too. If you've any changes to do I can make it. If you have questions, feel free to ask.

Hope it help.

Just dloading it now, I'll install and give it a try, thanks
Mooser