Machining Multiple Parts in One Setting

[bobby1]

Hello,
I have the set up for machining 12 small parts. I would like to know how to program BobCAD-CAM 2007 to machine these parts in one setting? Thanks in advance.

[tobyaxis]

Edit the Program to use G54-G59, or use G92. You could also use an Absolute Main Program and Incremental Sup-Programs to do 12 Different parts.

You didn't say what Machine Tool or Control your doing this with or what Level of V2007 your using. I'm using Level 2 Mill with the Base Predator 3D Simulator.

Personally I haven't gotten that far with V2007 to tell you if this can be done in a simple Predator SetUp.

Still getting used to the new U/I and G/U/I LOL.

Maybe you should call BCC Tech Support. I actually called today and spoke to a nice gentleman that helped a great deal.

Now I want to Modify the Post Processor and having a little trouble. With a little patients, time, mistakes, and Imagination it should workout nicely.

Sorry I couldn't be of much help


Cheers!!!!!!!

[skullworks]

Without a specific control - all advice is null.

Does your control support sub-programs or only 1 top down program?

G92 can behave strangely so if you are not aware of how it reacts on your control you might want to use G10 instead... Again, thats assuming your control supports G10.

There are about 20 ways to handle this... The way I have found works best for ME is to write each tool path as a separate sub program. Use the main to call the tool, set Sxxxx, call G54 G90 then call the sub, the next line (where the program jumps to after the M99 in the sub) has an M1. Next line has an N# as it is a restart point for the next part with that same tool. - repeat untill all parts are done then call a tool change from the main. - repeat -

Using a G10 to load the offsets means you can keep using 1 offset like G54 that updates each time G10 is used.

Inc subs also work and I use them all the time. Find whats most comfortable for you and easist on your control and least likely to get fouled up on a restart - (G92 can do strange things after a reset.)

This can be important because some machines... (Mazak) will not let you change an offset while in AUTO. So being able to start at any part with any tool is always the best method no matter how you deal with the positioning.

[dertsap]

easiest thing is to simply program for one part then you can copy and paste your program for multiple parts and use a g52 shift for each part or use subs with the g52 shift , either one is quite effective especially on fixturing that will be used again in the future , you will only need to pick up one w/s not twelve

[skullworks]

Again without a control...

G52 is an invalid command on Hurco, Okuma and Most Bridgeport controls to name a few.

[tobyaxis]

Originally Posted by skullworks Again without a control... G52 is an invalid command on Hurco, Okuma and Most Bridgeport controls to name a few.

Well sometimes we forget the important details LOL. Like Mazatrol AKA "No Control", LOL.

Maybe he will post back to tell us what CNC Control he is using.

[bobby1]

I forgot to say that my controller is FANUC OMD and that the BobCAD-CAM 2007 has the Level 2 Predator Software.

[tobyaxis]

Originally Posted by bobby1 I forgot to say that my controller is FANUC OMD and that the BobCAD-CAM 2007 has the Level 2 Predator Software.

Yes it does have Predator, but it is Level 3