Can someone check something out for me?

[MILLRUNNER]

We just recently installed MCX where I work and we had been running MC8 up until then. We use MC to post code for AGIE wire machines, and I have been having some trouble out of the code that MCX produces (or MCX's post processor). Sometimes when I post code from MCX, my wire macine won't take it. It will give me an error message - something like "unable to calculate beyond statement 04875". I will go back and post from the same file in MC8 and the machine will take the code it produces.

 

I got to thinking about it and I came to the conclusion that there were two different programs being produced by the different post processors, and I was right. MCX's program appears to be a little more precise, and the wire machine just doesn't like it. I am not sure if it is a setting in MCX itself or the post processor. I have the same program, both as text files, and I would appreciate it if someone could take a look at them for me and tell me what I need to change on the MCX side.

 

I can send them to youyr email. Thanks.

[Thad]

Upload them to the FTP. I'm not a wire guy, but I'm sure someone can help you out. Tell us what the file names are and what folder you put them in.

 

Thad

[MILLRUNNER]

I cannot upload anything from here at work. our internet access blocks things like that.

[Dave Ball]

email the files to me and I will put them on the ftp for you.

[MILLRUNNER]

I can't see your email adress Sheffer CNC.

[Dave Ball]

click on ShefferCNC to bring up my profile and then click on Click here to email this user. or just use this link

 

 

Email to ShefferCNC

[MILLRUNNER]

I still can't see anything. I have to use a proxy server to even be able to access anything, and I can't see half of the things that people see on the normal internet. I will just post the two programs here.

 

This one was created using mastercam 8:

 

N0100 G70 ;

N0102 G00 X1.17267 Y1.6905 ;

N0104 G90 ;

N0106 G01 Y-1.6905 ;

N0108 G03 X1.12672 Y-1.72761 J-.047 ;

N0110 G02 X.94049 Y-1.878 I-.18623 J.04011 ;

N0112 G02 X.75426 Y-1.72761 J.1905 ;

N0114 G03 X.70831 Y-1.6905 I-.04595 J-.00989 ;

N0116 G01 X-.12733 Y-.05132 ;

N0118 G02 X-.14097 Y.00545 I.11136 J.05677 ;

N0120 G02 X-.12718 Y.06253 I.125 ;

N0122 G01 X.70831 Y1.6905 ;

N0124 G03 X.75426 Y1.72761 J.047 ;

N0126 G02 X.94049 Y1.878 I.18623 J-.04011 ;

N0128 G02 X1.12672 Y1.72761 J-.1905 ;

N0130 G03 X1.17267 Y1.6905 I.04595 J.00989 ;

N0132 M02 ;

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

This one was created using Mastercam X:

 

N0100 G70 ;

N0110 G00 X1.17267 Y1.69019 ;

N0120 G90 ;

N0130 G01 Y-1.69019 ;

N0140 G01 X1.1673 Y-1.69081 ;

N0150 G03 X1.12674 Y-1.72753 I.00537 J-.04669 ;

N0160 G02 X.94049 Y-1.878 I-.18625 J.04003 ;

N0170 G02 X.75426 Y-1.72761 J.1905 ;

N0180 G03 X.71166 Y-1.69062 I-.04595 J-.00989 ;

N0190 G01 X.70825 Y-1.69038 ;

N0200 G01 X-.12733 Y-.05132 ;

N0210 G02 X-.14097 Y.00545 I.11136 J.05677 ;

N0220 G02 X-.12718 Y.06253 I.125 ;

N0230 G01 X.70825 Y1.69038 ;

N0240 G01 X.71165 Y1.69062 ;

N0250 G03 X.75424 Y1.72754 I-.00334 J.04688 ;

N0260 G02 X.94049 Y1.87801 I.18625 J-.04004 ;

N0270 G02 X1.12672 Y1.72761 J-.19051 ;

N0280 G03 X1.1673 Y1.69081 I.04595 J.00989 ;

N0290 G01 X1.17267 Y1.69019 ;

N0300 M02 ;

 

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

 

notice the difference in the preciseness of the decimal places. I think that is where the problem is. It will read a program posted from 8, but not X - which appears to be more precise.

 

How do i change the settings to make it where it does not post so precise?

[Chipmakr]

What kind of Agie machine do you have? We are running a Classic S and a Classic V here with MCX MR2 with no problems.

 

Have you looked at your NC tolerance in your control definition?

[MILLRUNNER]

we have (2) classic 2's. The NC tolerance in the control definition is what I think may be the problem. I don't know how to change it though.

 

MCX doesn't give me a problem most of the time, but sometimes it will give me the error message on really complex contours with a lot of radiuses in them. Like I said, I turn around and post it out of MC8 and it takes the contour fine. Those two programs above are for the same contour, but as you can see the one from MC8 is a little less accurate.

 

I am running Wire level 2 also.

[Chipmakr]

Close out all your open MCX files. Open a new instance of MCX and load your wire machine into the operations manager. Next open the “SETTINGS” drop down menu from the top of the screen. Now click on the second item from the bottom “CONTROL DEFINITION MANAGER”. Now under the “CONTROL TOPICS” field on the left hand side. Choose the top item “TOLERENCES” the top item on this page is NC precision. We are set to 0.000001 in both the inch and metric fields. What are yours set to?

 

I am sure there is a corresponding value at the machine as well for precision.

 

Can you eamil me the file and I will post it out here and send it back too you and see if it will run then?

[MILLRUNNER]

inch is 0.00001 metric is .0001. my email is [email protected]. Send me an email there and I will reply back with the files.

[Chipmakr]

Check your e-mail I just sent you over a zip file that we recieved from Agie that contains alot of traing documents.

[Roger Martin from CNC Software]

MILLRUNNER,

 

Open your MCX file. Expand the Machine Group Settings in you Operation Manager, select the Files branch, then 'Edit' the Machine, now click on the Control Definition icon in the toolbar and expand the Tolerances page and change the NC Precision settings. Remove one zero from the (Inch & Metric) NC Precision settings. Save those Control Definition changes and re-post the wirepath operations. Does this new NC look/work better for you machine? If so, (you can save this MCX to make the change permanent is this file) then you can make the change to NC Precision in your 'master' Control Definition for this machine. So these new setting will be used on a new wirepaths you create using this Machine/Control/Post combo.