[houdini]

hello, I am a newbie programmer, only been machining for a year now, but have been in computers and programming computers for 15+ years.

The shop I work at is using Gibbs CAM 2007 they dont pay maintenance and have a issue with post output running on our Milltronics VM16 and VM24 Centurion 6 I believe.

The post works good for everything except, they said they cannot use cutter comp.
It acts erratic they say, I havent tried it and they havent for years now, so I cant get a exact definition as to the issue, except that they cant use cutter comp.

Is there a way to get a newer post processor for these machines, ie like DL it from the net.
I thought there was a way to rewrite or write your own post processor, is it fairly easy or has some one already wrote a corrected one for these machines I can download.?
any help would be appreciated, these guys here can run Gibbs but they dont know much about computer programs.

Thanks guys
CHEERS!

[trevj1]

If the shop has a legit copy of GibbsCam, talk to the vendor about the post.

Cheers
Trev

[BOB SLACK]

check with milltronics, there are a few things in the controls that make them act a little strange with cutter comp..............one of them being " special flags" one of them is "trig help" and i cant think of the other one. they can switch them around and it will let you use regular cutter comp

[jpawelk]

Turn off the trig help feature. This can be done by using MDI and commanding 2 functions. The first command needs to be PB208=0 The second command is PB81=2 Sometimes this feature of the Milltronics control can cause undesired movements.

[Farmers Machine]

On my RH 30 when you teach the tools Z height you teach the diameter as 0 ZERO. In Gibbs you program with the cutter diameter you are using. Gibbs will calculate the tool path with cutter comp in The G code. In the Gibbs set up page you have lead in and lead out, if this distance is shorter than the radius of your tool diameter it will cause cutter comp on the CNC to act stange. By setting the diameter at 0 on the control you can tweek in endmills by .001 or .002 on the paramater/ tool page to get exactly on size and the control will pick up this small diameter on the lead in move to the geometry.
Good Luck
The Farmer.

[Robdwatts]

Hello,
I'm having a problem changing pocket processes to contour processed to open machinging markers. Can anyone help me with this part of the programming?
Thank you
Rob

[Tim Horgan]

Try setting Misc parameter "90 Degree Cutter Comp" to YES. This makes cutter comp on/off work more like other controls. Might be the "erratic" that your referring too…

This parameter was added 6/24/09 version #255

[houdini]

Ok so I'm clear as to what I want to. Be able to do is turn on cutter comp in Gibbs and be able to adjust the radius in the machine tool diameter and have it mill correctlym
Do any of these solutions mentioned hear cause me to be able to do this?

[houdini]

Try setting Misc parameter "90 Degree Cutter Comp" to YES. This makes cutter comp on/off work more like other controls. Might be the "erratic" that your referring too…

This parameter was added 6/24/09 version #255

I dont know where your talking about Misc. parameter? I dont see it in Gibbs, or are you talking the mill?

[houdini]

On my RH 30 when you teach the tools Z height you teach the diameter as 0 ZERO. In Gibbs you program with the cutter diameter you are using. Gibbs will calculate the tool path with cutter comp in The G code. In the Gibbs set up page you have lead in and lead out, if this distance is shorter than the radius of your tool diameter it will cause cutter comp on the CNC to act stange. By setting the diameter at 0 on the control you can tweek in endmills by .001 or .002 on the paramater/ tool page to get exactly on size and the control will pick up this small diameter on the lead in move to the geometry.
Good Luck
The Farmer.

OK Im unclear as to what setting your talking about. Gibbs setup page, what page, the operations page for setting up a process? Do you mean the entrance and exit parameters?
Setting the diameter at 0 on the control, what control, the tool radius parameter on the machine or the tool diameter in the tool dialog in Gibbs.

Heres what I want it to do, setup a mill path in Gibbs say .5 cutter add .002-.003 to stock, post and run file. measure for difference needed and change that difference in the tool diameter parameter in the mill and rerun the same program, not have to readjust the Gibbs file. Mainly I want to do this for trying to better match multiple tools for say squaring off a corner where a larger endmill was used and a smaller one is used to clean it up, and adjusting for the differences in the tolerances in the endmills, all in all to be able to use reground endmills also.

[von007]

Originally Posted by Tim Horgan
Try setting Misc parameter "90 Degree Cutter Comp" to YES. This makes cutter comp on/off work more like other controls. Might be the "erratic" that your referring too…

This parameter was added 6/24/09 version #255

I dont know where your talking about Misc. parameter? I dont see it in Gibbs, or are you talking the mill?


Yes he is talking about the mill....cent5 6 or 7 same same
go to main pg on crt para misc. u may need password= PROTO access level 3

von007
Chips AHOY