Assuming code of..

Main Program in Absolute:
...
G90 G0 G54 X0 Y0
G43 Z1. H1 M08
M98 P2
...

Sub Program in Incremental:
...
O2
G91
G99 G81 X0 Y0 Z-1.05 R-.9 F30.
X1.
G80
...

How deep, Absolutely, should the tool go?

Z-1.05
or
Z-.05

'Rekd

The way i read what u have from Z zero you would have drilled
1.95 deep

Z-.050 is how deep!



Main Program in Absolute:
...
G90 G0 G54 X0 Y0
G43 Z1. H1 M08 ( move to Z1.0 abs)
M98 P2
...

Sub Program in Incremental:
...
O2
G91( turn on Inc, moves now Inc from here)
G99 G81 X0 Y0 Z-1.05 R-.9 F30. (feed down Z-1.05 from Z1.00 = Z-.050)
X1.
G80

Originally posted by fjd
The way i read what u have from Z zero you would have drilled
1.95 deep

Note the G90 in the MAIN program and the G91 in the SUB program. So is it reading the R-.9 then taking the Z-1.05 from R-.9?

WMS, this is what I thought also. But according to the (thank god) Z over travel alarm I recieve just above the part, it doesn't.

The max travel on the Z is almost 3/4" BELOW the top of my part, the tool is set to the top of the part, (.04" thick part)

'Rekd

The dangers of incremental proggramming.:( :(
Always use abs. even back in the days of manual
programming. It pays to take a little extra time.

PEACE:D

Originally posted by hardmill
The dangers of incremental proggramming.:( :(
Always use abs. even back in the days of manual
programming. It pays to take a little extra time.

PEACE:D

True, but the file size can be a *****, 'specially with 268 parts on a 12 x 12 sheet.

The code is from a MC post. Using Abs subs makes the code longer than without subs. :rolleyes:

'Rekd teh breaks out the MPost handbook.

Matt,

This gets even stranger!!!:confused:

I just ran a test on a vf2 software ver 9.62n

And here's what happens with your code.



Main Program in Absolute:
...
G90 G0 G54 X0 Y0
G43 Z1. H1 M08 (OK here, moves to Z1.0)
M98 P2
...

Sub Program in Incremental:
...
O2
G91
G99 G81 X0 Y0 Z-1.05 R-.9 F30. (here's where it get weird, it moves to Z.100 abs which would be right, Z1.0 abs - .900 inc = Z.100 abs, then it drills to a depth of z-.950 abs. Were did that come from?)
X1.
G80


I'll try a newer version of software when another machine is free, they are all running right now.

I have never run into this as I have never programed a drill cycle with incremental code.

Any use in throwing macros on the table?:confused:

Hey what ever happened to the file you were sending me?

PEACE:D

I sent it one day, and it came back the next day, (the day we found out we didn't get that job)

I don't have macros on my machines. :(

'Rekd

Perhaps next time:p
Send me an email again. I know I responded to one of yours.
Maybe the server was down that day.

PEACE:D

I believe it's moving inc. -1.05 from the z.100 absolute which takes you to z-.950. Could you change the z value from -1.05 to however much you actually need it to go--the depth of the hole or the thickness of the part plus the .1 that it is above the part?

Originally posted by brtlatjgt
I believe it's moving inc. -1.05 from the z.100 absolute which takes you to z-.950. Could you change the z value from -1.05 to however much you actually need it to go--the depth of the hole or the thickness of the part plus the .1 that it is above the part?

I'm beginning to think that is what's happening. (Not at work right now, but will look tomarrow). Seems it's going from
Z1. Abs
Z.1 Abs via an Inc R-.9
Z-1.05 from the last position at Z.1 Abs

I'll have to tweak my post or change my programming method. I program the tool depth in Abs mode, but do the Xform in Inc subs, and would prefer to keep it that way for harmony and lack of confusion.

Thanks for all the input!

'Rekd still learning after all these Rum & Cokes

Originally posted by brtlatjgt
I believe it's moving inc. -1.05 from the z.100 absolute which takes you to z-.950. Could you change the z value from -1.05 to however much you actually need it to go--the depth of the hole or the thickness of the part plus the .1 that it is above the part?

Exactly right! Couldn't see the Forest for the Trees!
Thanks for cutting them down.:D

And Now that makes perfect sense, Dumb machine anyway, did exactly what it is supposed to not what we humans think it should.:rolleyes:

you guys are scarein' me here.
Somebody take the keys outta that machine :D

Hi All,

Where can I find a reference/tutorial on g-code?

Thanks,
bb99

Originally posted by bb99
Hi All,

Where can I find a reference/tutorial on g-code?

Thanks,
bb99

I searched for g-code reference on google (http://www.google.com/search?q=g-code+reference&sourceid=mozilla-search&start=0&start=0&ie=utf-8&oe=utf-8) and MSN (http://search.msn.com/results.asp?RS=CHECKED&FORM=MSNH&v=1&q=g%2Dcode+reference) and found several sites.

'Rekd teh :drowning:

It helps to search for the right thing. I was searching for "g-code standard" which was not getting me what I wanted. I found references to "Gerber RS-274D/X" which, I guess, is the name of the standard. But, I could not find the standard it self!

Thanks for the push in the right direction!

bb99