V21 . cut depth off by amount of safe height

I have 2 suites of v 21 .
1 on my lap top - works good.
2nd one on computer in the shop.

I have compared both back and forth and can't seem to figure this out.

The 2nd one,
when you want to have a complete z cut depth of .5" and a tool safe height of .1" the last z movement is .6" (it adds the 2 together)

My cut depth is set as a negative and the safe height is set as a positive.

What are your thoughts?

Thanks!

Maybe I am missing something, but this sounds correct to me.
You have told the machine to cut 0.5" (that is 0.5" down from Z=0) or a negative Z. You then want the tool to return to safe Z which you have defined as +0.1". The distance between -0.5" and +0.1" IS 0.6"

Quote:

---

Originally Posted by GBowes

Maybe I am missing something, but this sounds correct to me.
You have told the machine to cut 0.5" (that is 0.5" down from Z=0) or a negative Z. You then want the tool to return to safe Z which you have defined as +0.1". The distance between -0.5" and +0.1" IS 0.6"

---

Only in incremental mode.

Take a look at this .
Just a simple 2inch long cut.
Programed to a depth of cut of .5" deep.
Top program does it correct (lap top computer)
Bottom program does it too deep ( shop computer)

***(Check out line N80)***

(This one is from my lap top)

N10 G17 G20 G40 G49
N15 G55 G80 G90 G94
N20 G53 G0 Z0
N25 X0 Y0 M5 M9
N30 (2 inch line at .5" depth,Load Tool 1)
N35 M0
N40 T1 M6 G43 H1
N45 S1000 M3
N50 Z0.1
N55 X1.
N60 G01 Z-0.25F1.5
N65 X-1. F8.0
N70 G00 Z0.1
N75 X1.
N80 G01 Z-0.5F1.5
N85 X-1. F8.0
N90 G00 Z0.1
N95 G53 G0 Z0
N100 X2 Y2 M5 M9
N105 M2


(This is from the shop computer)

N10 G17 G20 G40 G49
N15 G55 G80 G90 G94
N20 G53 G0 Z0
N25 X0 Y0 M5 M9
N30 (2 inch line at .5" depth,Load Tool 1)
N35 M0
N40 T1 M6 G43 H1
N45 S1000 M3
N50 Z0.1
N55 X1.
N60 G01 Z-0.25F1.5
N65 X-1. F8.0
N70 G00 Z0.1
N75 X1.
N80 G01 Z-0.6F1.5
N85 X-1. F8.0
N90 G00 Z0.1
N95 G53 G0 Z0
N100 X2 Y2 M5 M9
N105 M2

If you are using the same part file to post with and I mean taken from one computer to computer without change, then it is the post processor. Copy the post processor from the laptop and replace the one on the shop computer.

It should be the same then.

Mike

Same post prcessor.
They used to do the same output but somewhere along the lines I must have goofed it up.

Any idea's where ?

Airchunk

go back to setup
under drivers general tab
make sure incremental xyz is (not) checked should fix it

dw

Hmm , good idea .
I will go check !
Thanks

dwood
Thanks so much!!!
You NAILED it!