MastercamX and Haas VF2 issues

[X7racer]

I have Mastercam X and a HAAS VF2 machine, I have a few problems with it writing the G code out to the machine.
First problem comes when initiating Mastercam to write the G-code, I get a error message that says, "ERROR- WRITE NC OPERATION INFORMATION MUST BE ENABLED IN CONTROL DEFINITION - SET AND REPOST" This error message comes up during "initiate opening post processor file(s)", I press "ok" the only option available and it continues doing it;s thing opening the NC editor. What does this mean and where do I go to change this so this message does not come up anymore?
Next problem after loading the NC editor is in the G-code itself, here is a typical sample.

N100 G20
N110 G0 G17 G40 G49 G80 G90
/ N120 G91 G28 Z0.
/ N130 G28 X0. Y0.
/ N140 G92 X14.4959128 Y11.4986376 Z10.
N150 T1 M6
N160 G0 G90 X-.99 Y.0101 S2444 M3

Problem I am having here is that I will get on the VF2 a out of range error on either line N130 or N140 and more frequently at line N160 , or the machine will go off onto another area of the table and start machining in the wrong area, even after setting up the G54 coordinates in the machine. Now if I use Bobcad/cam it uses G54 and all is fine, but not with Mastercam. I have tried to change various coordinates in mastercam but haven't found a solution to this problem.

The next area of of concern is how many lines of code mastercam generates to do simple operations, most of my operations I do is boring a few to 8 holes in a single piece of stock, hole sizes vary from 1.35 to 3.5", for example I had 3 through holes to bore in a solid piece of cold roll, 1.68", 1.75" and 3", simple just drill and bore, but mastercam came out with 62,530 lines of code, and when I went to load this into the machine it ran out of memory. Why doesn't mastercam simply use the G85 codes and do this in less then a dozen lines?

Ok one more thing at the moment, and I really appreciate the help I get from this community. Instead of stamping my company name on my products, like I have been for years, i have been told that I can use the VF2 to do my engraving for me. ok fine, so in mastercam I will give it a try, however when I do the toolpath for engraving I get a error message stating, "your mastercam maintenance contract has expired", and then proceeds to go through the toolpath as needed and seems to come out just fine. Is this anything I need to be concerned about, it seems to function fine.

Software is Mastercam X mill level 3
My post processor is "Generic HAAS 3X VMC"
Machine is a 2001 HAAS VF2 3 Axis

Again thanks for the help, and hopefully soon I will be able to be proficient enough to help out others here.

[PBMW]

You have multiple issues going on.
You need to look at your Misc intigers on the misc values tab on the first page of an op parameters window. You will find I think that misc integer #1 needs to be a 2 to get G54's and then you can change the offset in the planes tab.


The three block delete lines are caused by the misc integer issue.

You need to set up your machine def and your control def. Call your reseller if you don't know about this.

I have a hard time believing a drill and bore routine can be 62k of program.
I could believe it if you were interpollating...
If you want to use caned cycles...turn them on in the machine def and in the post. Once again, if you don't know how, call your reseller.

And ...apparently, your maintanance has expired.
There isalso a lot of help to be had on the Emastercam site.

[ljagger]

Hello X7racer, You can fix the "ERROR- WRITE NC OPERATION INFORMATION MUST BE ENABLED IN CONTROL DEFINITION - SET AND REPOST" message by going into the "Machine Definition Manager" then select the Edit Control Definition Icon. when there, under the Control topics select the Files topic. On that page you will fine a check box that says NC paramter file. Make sure that you have a check next to the Write NC operation information. Also make sure that just below that the Source ops parameters only is selected. This shoud get rid of your eror message.

I have also reworkd a .pst file that i use on a VF-1, VF-2, VF-E and a TM1P that seems to work much better. I can e-mail this to you if you'd like to try it out.

Lyle

[X7racer]

Thanks for the responses. It took me awhile to get back here cause I have been out of town.
Most of the information has been very helpful and corrected most of the problems I have been having.
As for the response of contacting my reseller, I have none, I bought the VF1 and computer which came with the mastercamX as a package deal. When contacting a rep from Mastercam, they seemed more interested in selling me the new version or purchasing other licensing items from them.

As for the 62K lines of code, yes interpolating is the way I was told to use this machine for the close tolerances I need for the type of work I am currently doing, if anyone has a better way of keeping <1000th on bored holes I would greatly appreciate it. So far I have been using a lathe with a bore hone to maintain this tolerance.

ljagger, I would like to see the post you have modified for your VF machine.

Thanks for the tips.
Dave

[maxine]

Originally Posted by ljagger Hello X7racer, You can fix the "ERROR- WRITE NC OPERATION INFORMATION MUST BE ENABLED IN CONTROL DEFINITION - SET AND REPOST" message by going into the "Machine Definition Manager" then select the Edit Control Definition Icon. when there, under the Control topics select the Files topic. On that page you will fine a check box that says NC paramter file. Make sure that you have a check next to the Write NC operation information. Also make sure that just below that the Source ops parameters only is selected. This shoud get rid of your eror message. I have also reworkd a .pst file that i use on a VF-1, VF-2, VF-E and a TM1P that seems to work much better. I can e-mail this to you if you'd like to try it out. Lyle

Would it be possible to get a copy of the post file?