Need Help!- V-21 G-Code Question

[SteveS]

My use is 2-D and in the past have used the approach depart feature. Now I am cutting in the surface and am having a problem with the tool ramping out and cutting the surface where I don't want it to. Below is a segment of code.

The G0 Xxx Yxx Z0.0000 takes it to the next cut location by a 3-d movement and Z doesn't get above the surface first. This creates what appear to be scratches on the surface.

My elementary solution is to edit the G Code by making separate lines for G0 Z0.0000 and then put X Y on the next line with its own G0. A lot of manual work.

Is there a method in BobCAM G Code creation that I can use to force Z to happen prior to X Y movement?

T1 M06
G71
G0 X54.4545 Y146.7227
G1 Z6.350010
G2 X57.4419 Y139.7061 I-6.7462 J-7.016620
X52.4606 Y131.2115 I-9.7336 J0.0000
....
X54.4511 Y146.7259 I0.0000 J-12.4204
G1 X54.4545 Y146.7227
G0 X55.9467 Y150.6218 Z0.0000
G1 Z6.350010
G2 X58.5698 Y148.1049 I-9.7499 J-12.786820
X61.5792 Y140.2267 I-10.0750 J-8.3625
...
X49.0233 Y162.5631 I0.0000 J-7.8784
G1 X49.0245
G0 X49.0233 Z0.0000
G1 Z6.350010
G2 X51.1181 Y160.9506 I-0.7839 J-3.185320
...
G3 X50.3321 Y154.9616 I3.0342 J-3.3314
G0 X56.6313 Y161.6334 Z0.0000
G1 Z6.350010
G3 X53.8925 Y165.6291 I-14.1277 J-6.747120
X53.8166 Y165.7054 I-1.4549 J-1.3723
...
X73.3262 Y101.6735 I0.0000 J-0.8300
G1 X76.7529 Y95.5067
G0 X76.8139 Y95.4916 Z0.0000
G1 Z6.350010
G3 X80.9599 Y94.9167 I4.6314 J18.163120

Thanks in advance - Steve.

[BurrMan]

This is done with your post processor. You'll have to tell what post you are using then someone can tell you how to edit it to output the ending values in the order you want.

[SteveS]

I went back and manually broke all the G0 lines into two, with the Z move first.

Cutting went fine. Will contact BobCad on how to change the post processor.

It actually seems odd that any post processor would have that mode. I'm only cutting wood and that could be a real problem with metal.

[Allen123]

You can always use your tool up and down prior to any cutting. This way you have a z move first.

Try that

[SteveS]

"You can always use your tool up and down prior to any cutting."

My situation was in selecting several (9) chains and then using Auto in the Machine tab to generate the g-code. When moving from one chain to another the path was just a ramp which cut notches where I didn't want. The generate went to Z zero to start each chain, but didn't go to Z zero at the end of the chain.

I'm kind of following your theme. I named each chain as a layer and now Auto each one seperately in the Machine tab. That way Z goes to zero each time before the x-Y movement. This actually helps with organizing the sequence of chains to minimize haphazard travel with the other method.

If I ever get really annoyed, I would try to write a macro that takes the chains in alphabetical order with a tool up between each one. Never wrote a macro in BCC before.

[moldmker]

Looking at the code from your 1st post, does your machine feed into the work with a Z positive number?
If so, I can see where this would require some special scripting.

Standard controls feed down in a negative Z, Bobcad has no problem generating Cut Auto code for this format.

What control is this and did Bobcad have an exact post available?

moldmker

[SteveS]

Moldmker,

My machine is a German design with unique controller. I bought it turn key for a good price, but yes the Z is a positive value. Also serial cable connection.

BCC provided me a unique post back in Version 17.

If the Z was negative or positive, the ramp out would still be there with this post when multiple chains were coded as Auto.

I'm going to change controllers in the next 6 months which should solve or change the problems.

[HMB3000]

your machine is just like a flexicam route for posting...I had Bobcad write a few post when I was programing a Flexicam a few years ago.you might want to look at the try Flexicam.exe
http://www.bobcadsupport.com/posts/i...dsupport/posts

[Allen123]

Connect at Z:

This is a good feature if you are working with more than I chain. If you want to control the up and down and in between's of chains you can use this feature.

It will chain all your tool paths together and set the clearance for those chains.

What about that?

[SteveS]

Allen,

I just tested with a couple generic chains, generated the g-code and it seems perfect for what I want. Being in the 3D pull down, I never saw it. I'll try cutting later today.

The code looks a bit more efficient (shorter).

Thanks a lot.

Steve.

[Allen123]

Originally Posted by SteveS Allen, I just tested with a couple generic chains, generated the g-code and it seems perfect for what I want. Being in the 3D pull down, I never saw it. I'll try cutting later today. The code looks a bit more efficient (shorter). Thanks a lot. Steve.

Yup that's a cool feature that will do what you want. Glad I could help!