GearHeads Corner

Here's a couple of suggested changes to the cam module.

M3 and M5 post after each machining operation even though the same tool will be used for the upcoming machining operation. This causes the spindle to wind down and up again unnecessarily. Normally M3 is only seen after a tool change and M5 is only seen after all machining operations are completed for the tool currently in the spindle.

The G43 and H are missing from the tool change line so the tool offset is not applied.
Tool change should be:
T1 M6
G43 H1


Would it be possible to add drills to the type of tools available in the cam module? This would allow the center holes of gears to be drilled and reamed for perfect alignment.

Thanks,
Kerry Harrison

Kerry:

Good idea's all. I will look into them for next release..

ARt

Art:

I do not understand the particulars, but the symptom described (viz., spindle wind down and up) sounds similar to what I experienced but I wasn't changing tools.

Brian.

Hi Guys:

  Fixed for next version. The spindle will not cycle unless a tool change actually happens. Also, the post allows for a G43H1 or whatever youd like. Will probably be out tomorrow.

Thx
Art

Hi Art,

Version 2.259 now posts two M5 commands between machining ops so the spindle will turn off and stay off after the first op is completed.

I am not understanding your comment regarding the G43 H1 line. Is there some way I should make the post include G43 H1 after the T1 M6 line?

Thanks,
Kerry

Kerry:

  Ouch, I must have forgotten to include a new post file.. Ill check what happened
and respond..

Thx
Art

Kerry:

Fixed and uploaded. Sorry about that, I missed a line that shunts in an extra M5. Its gone. It is now properly posted at the end of all jobs.  As to the G43H1, it is now in the defaultmill.pst post file, so if you use the standard post it should now give you a G43H1 after any tool change.  You can stop this by editing the defaultmill.pst post file or creating a new one that doesnt post that message.

Thx
Art

Art,

Yep M3 and M5 now post as they should, almost. There is a M5 at the beginning of the code that is not needed but since it is followed by M3 the spindle still starts properly.

The tool change code still needs a bit of work. I apologize for not explaining the tool change code in more detail previously. The H number must be the same as the T number. Here's why. The H number applies the tool offset. It must be the same as the T number so the tool offset stored in the tool table for each tool will be applied to the tool in the spindle.

Examples:
T2 M6
G43 H2

T5 M6
G43 H5


Another thing that's missing is M30. This should be the last line of code. M30 is - End of program, with return to program top.

Thanks,
Kerry

Hi Kerry:

  My appologies, that was a typo, the H word was typed in as a 1 instead of a %d internally, so its always a 1.
this has been fixed for next release ( probably today..). Ill make sure an M30 is there as well. I have one in my epilog
so I hadnt noticed it missing..

Thx
Art

Looks good now Art. Now the tool changes will work properly on my Tormach, Milltronics VMC and lots of other machines I bet. - Thanks

Here's another thought.

Along with making drills available would it be possible to have an option where the center of the gear hole would snap to or somehow be precisely positioned at XY zero (or other exact locations for that matter) on the workbench? This will make set-up really simple and fast. Just find the middle of the stock, zero the machine at that point and you're ready to go. It seems to me this would be particularly useful since so many gears are round.

Thanks again,
Kerry

Kerry:

  That option already exists. If you use the options and select Center as your origin, when you send a gear to the
workbench, it will center the shaft hole on 0,0.  This shoudl work for all gears as I always make the shaft center 0,0 on all gears.

Art