Post Problem @ High School

[CNCTitan]

Greetings,

 

I'm providing tech support for a high school. We have Mastercam X, Mastercam 9 and a Techno DaVinci (EP1090). We recently had a hard drive crash and had to reinstall everything. We also recently upgraded to Mastercam X and are trying to do the projects in the Mastercam X CNC Curiculum books. The instructor has very little formal training on Mastercam and I have none.

 

We're having a problem at the start and finish because the bit is not clearing the workpiece at the start and end of the run. ie. The bit isn't retracting when going to the first XY coordinate and isn't retracting when going home. The students have broken a couple of bits. I did get updated control, post and .rmd files from techno as I was hoping that was the problem. We still have the bit dragging across the work surface going to the first point and going home.

 

The problems with the Mastrcam X produced .NC files seems to be that it goes to the first X/Y coordinate and then retracts.

%

G90 G80 G17

T230 M06

S18000 M3

G0 X.3841 Y.8696

Z.25

Z.1

G1 Z-.125 F100.

G2 X.4018 Y.8962 I.0942 J-.0435 F200.

G1 X.3663

 

If I process the same file with Mastercam 9 I get the following.

%

WCS: TOP

G0 Z2.505

G90 G80 G40 G17 G00

X.3211 Y.8261 S10000 M03

Z2.5

Z.1

G1 Z-.125 F100.

Y.0313 F200.

X.447

 

Is there a setting I'm missing?

 

Thanks.

[produca2]

The retract value seems to be missing? or are your tool length ofsets set corectly at the machine? could be a bunch of things as I am trying to understand your question.

[Steve Biehl - Cimquest Inc]

looks like a custom post edit to put the Z move before the startup odes. If you have the V9 post, in X go to Settings, Run User App and run the Updatepst application. That will update the old post to X.

[Kannon]

Maybe check the clearance tab..use clearance only at start and end of operation..its under contour parameters if thats what your using...I am using version 9...put your clearance height at..2.505

[CNCTitan]

I converted the post file from Version 9 to X. Looks like that should do it.

 

Below is text from the Version 9 file. My guess is the version 9 had a fix for the setup we have(5+ years old) that isn't incorporated into the X post that the company sent me. I'm also assuming the problem we had counts as a 'tool crash'.

 

# 03/19/01 msf 1. Post now calculates the maximum z value and adds .005

# and outputs that value as the first move.

# This should take care of tool crashes when the machine

# homes all axis and starts the program at z zero.

# 2. Change the following line to add a clearance to the most postive z move.

# This will help with the referance return problem with Techno

zmx = (z_max$+0.005)# Most positive z + .offset value

 

Impressed with the quick turn around on the forum.

 

Right now I'm helping the teacher do the cookbook stuff. Any recommendations for learning more once we get beyond the basic curriculum? ie. We currently set things the way the book tells us but don't necessarily know why.

[Philcott]

Titan,

 

Taking a course from your local mastercam reseller would be the first thing to do. After that I would try to find a local mastercam user who might be willing to become a mentor to the school. I often help out the teacher at our local high school as a service to my own community. He would be able to explain the how and why of the different screen fields.

 

This is a powerful piece of software but you do need to know what each field does and when to use it or not.

 

Also by posting here you have discovered the best resource to be found. Treat folks well and you will be hard pressed to ask a question that we don't climb all over each other to answer.

 

Welcome to the forum. Lets keep those kids from crashing the mill.

 

Phil

[Todd Tracey from Fastech]

Most of the Davinci's go to X, Y , Z zero at the start and end of the program by default due to a setting in the router control software. CHanging the post won't fix it. Check with the Techno manual or Techno dealer for the correct settings under the setup page.