Retract after a specified machining time

[jaydenn]

Morning,

 

Does Mastercam offer the ability to set a "retract after time" value?

For example, I'm going to mill a large pocket with WG-300 ceramics, and I want the cutter to retract and stop every 3 minutes for edge rotation.

 

Is it possible to automate this?

 

J

[gcode]

Yes.. the new high speed toolpaths have a switch on the Tools Parameters page that allows you to define

distance or time in cut as a retract parameter

To function properly, your post processor will require some editing

[brandon b]

What version of mc did this start?

[Guest]

X3'ish I think, it started to be implemented

[jaydenn]

Thanks,

I see that now.

However, It's useless without post editing.

How am I to distinguish the time based retracts? Where will I start editing?

 

J

[gcode]

this is the meat of it

 

 pxout, pyout, pzout, pcout, [if gcode$ = 1, `feed], strcantext, scoolant, e$

 

from here down

        if cur_cflg$ = 70000, tool_chk = 1
      if cur_cflg$ = 70000,
              [
              pbld, "M09" ,e$
              pretract0, e$
              pbld, "M00", "(TOOL INSPECTION POINT)", e$
              pbld, n$, *sgcode, sgabsinc, pwcs, pfxout, pfyout,e$
              pfspindleout, e$
              pbld, n$, "G43", *tlngno$, pfzout, e$
              pbld,*feed, *scoolant,e$
              tool_chk = 0
              ]

 

this needs to be added to these 2 blocks

 

prapidout       #Output to NC of linear movement - rapid 

 

plinout         #Output to NC of linear movement - feed

 

 this is taken form a 4 axis mpmaster post

[brandon b]

I was thinking of a different problem I had years ago.

 

Wanted tool inspection at approx. One hour but only retract when the cutter is off the part.

[AMCNitro]

Yes.. the new high speed toolpaths have a switch on the Tools Parameters page that allows you to define

distance or time in cut as a retract parameter

To function properly, you post processor will require some editing

Not that I need it but now im curious.  I cant see it, screenshot?

[gcode]

I've used it a lot with high speed rest roughing and a time interval setting

It's pretty smart about where it pulls up. 99% of the time its at the end of a cut where it would normally retract.

Its very useful for long roughing programs

instead of 50 or 60 15 minute toolpths.. and all the work it takes to make them

you program 1 toolpath and set a retract interval.

If experience shows the interval can be longer ( or must be lower), you just change the setting and repost

[jaydenn]

Thanks a ton GCODE.

I got it working perfectly.

 

J

[gcode]

screen shot... see attachement

 

 

tool inspection.pdf

[jaydenn]

Afternoon Everyone,

I need to resurrect this topic.

 

I thought it worked, but it doesn't. Or should I say, it works in typical "Mastercam" fashion!

 

All jokes aside;

When I use a "surface high speed" operation, and I turn on the "tool inspection", everything works wonderfully.

 

Now, when I use a "2D high speed" operation, and I turn on "tool inspection", it doesn't work at all.

 

I've compared the NCI for both of these paths and only the "surface" version has the 70000(pause for inspection) control flag in it.

 

Is this yet another mastercam bug?

 

The 2D path is actually generating the retract points per my criteria, but it doesn't output the NCI flag to initiate the pause.

 

How can I remedy this? I'm really, really, really counting on these inspection points to work!!!!!

 

Jay

[crazy^millman]

Might need to do a nci search and dig into the NCI using some logic searches. PM Colin he is the person I would think that could give you some good insight.

[mikenaturalice]

I think it is a post/machine issue, not really a mastercam issue. I think the last time I used that feature I got the M0 after the retract, but no spindle code afterwards so I had to manually edit that in. BUT, I think that was in X3-X4, no idea how well it works (or doesn't) now....