Cutter Compensation on Haas Mini Mill

[Gouger]

I am trying to locate a POST for the Haas Mini Mill (VF series) that will produce code for cutter comp. correctly. Cutter comp only works in the XY plane and needs to be set during a linear move. I get alarms from the cutter comp being set during a G2 or G3 move using the HaasVF post as well as most other posts that I have tried. I have the comp OFF in the COMPUTER and LEFT in the CONTROL using version 7.2 Does anyone have any suggestions? Thanks.

[Gouger]

I may have solved my own problem. I have to try it still. I noticed that my leadin/out straight lines were 0 in length. Making it start with an arc. I am going to add some length to this line making the CUTTER COMP do a G1 move before the G2. I hope this is the solution. If there are other tips, please let me konw. I am still learning the ropes here.

[Kenneth Potter]

Iv ran in to that problem before & the lead in lead out at least when i tryed it with cutter comp was a bit tricky . I found that the machine control look ahead detects a possible gouge if comp is not complete be for contact with your machining profile. therefore getting a fault "fanuc 0M controls" . This gouge wont show up in mastercams simulate c-comp backplot. If i remember correctly cutter comp must on at linear lead in not the arc lead in. & off at the linear lead out.

Hope this helps

Regards

Kenny

[This message has been edited by Kenneth Potter (edited 11-17-2000).]

[Kenneth Potter]

Oh yea make sure that you have the patch update installed.

" Ctour8.exe "

[Gouger]

Is that patch for version 7.2? Thanks for your input.

[Kenneth Potter]

No thats for ver 8.0 "sorry bout that " But check & see if you have all the latest patches for 7.2c

[PBoulanger]

Your right Ken. Most Fanuc controllers I've used require a linear move in order to engage cutter comp., so Robin you do need to add a linear distance to your entry move. Just remember to make it equal to or greater than the radius of the tool you are using or you might get an alarm on your controller.

Hope this helps.

------------------

 

[Gouger]

I have been programing with COMP LEFT in CONTROL for my profiles since the HAAS uses cutter comp. Do you have any preferences for the COMP in COMPUTER settings?

[Kenneth Potter]

Comp in computer option is totally up to you. sometime i use comp in control & computer so that my diameter register value in the control reads zero. then the operator can add A positive or negative direct value for tool wear. "ie" tool dia is .25, Comp in control & computer on. Dia register value = 0 . Now part conture checks .01 Undersize

Operator adds this value to the Dia register D1 -0.0100 . Now part checks Zero