mazak/mastercam co-ords.

[greybeard]

Hello-as I knock quietly on the sites door and poke my head inside. Been shadowing the group for quite awile-reading,watching, learning. Great resource. Now I have a question-hoping for guidance. I'm new on a mazak VMC and want to feed it from our Mcam, V8.1. I have done a pocket-verified it and posted it-saved it as a .EIA. Now I program the machine-touch off my part 0,0,0 with the probe-the call up the EIA as a sub-program. The machine rapids to the back right corner-then errors out. Figuring the co-ords are not in synce. So-the question is-do I obtain my actual co-ords from the probe and enter them into the mastercam fields-then verify and post? Or do I do some other magic?

[Bruce Caulley]

Sounds like you have a G53 in the top of your programme. If you have set your 0,0,0 with a G54-G59 offset then you will need to have this at the beginning.

 

Bruce

[Jack Mitchell]

The quickest method would be to use a Mazatrol program containing your WPC. This can be auto or manual probed.

Branch out to the EIA program without a G54.

 

The smarter method requires you to probe in Mazatrol and write down these numbers, then input the G54 values as the same.

 

The wisest method would be to use an edge finder and to teach in each value field.

 

I don't believe auto or manual probing is possible in EIA on a Mazak vertical - I could very well be mistaken. Hang in there I am sure others will contribute with a response.

 

 

Regards, Jack

[IntegrexMan]

Auto probing your G54-G59 is possible in EIA. Are you using a Renishaw probing system? Do you have the manual for it? There are exmaples in their as to how to output to G54.

 

Craig

[dan m]

quote:

---

The quickest method would be to use a Mazatrol program containing your WPC. This can be auto or manual probed.

Branch out to the EIA program without a G54.

---

That's the way we do it here. mazatrol wpc is our main programs mastercam puts out our sub programs.

[greybeard]

Ok-lots of input to get me headed in the right direction-thank you all. I do use the renishaw in mazatrol auto to locate my part. So if I get this right-I am to manually edit my post to eliminate the G54 code. I work nights-so it will be later today that I can get inside the post to see what is up. Thank you

[greybeard]

Got some info phoned to me from work.

 

 

O1(PROGRAM - 1)

(DATE - 21-02-05 TIME - 14:53)

N2

G20

G0G40G80G90G94G98

G0G28G91Z0.

G0G28X0.Y0.

( 1/8 FLAT ENDMILL TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - .125)

T2M6

G0G54G90X-.3844Y-.5462S6000M3

G43H2Z.25M8

Z.1

G1Z-.03F6.16

G2X-.3938Y-.5625I-.4523J.2502

 

 

The probe returns these values for the corner of my part:

X=-28.4765

Y=-9.1061

Z=-23.8382

 

Are you saying to overwrite the x-.3844y-.54625 values?

[Jack Mitchell]

X=-28.4765

Y=-9.1061

Z=-23.8382

 

These are the values that you must enter at the G54 thru G59 offset screen.

Push the main menu screen at the control twice (upper left) ~ from here you will acsess the offset screen, I think it's the third button in.

 

The Mazatrol WPC unit is an entirely different beast.

 

Regards, Jack

[greybeard]

Thanks Jack-just getting started with the Mazak-so much to learn. Will get to it tonight.

[Sparky112]

JMain,

we do alot of combination prog.'s on our mazaks. weve found that if not rerunning specific tools is ok than run MC as a sub program with WPC in main and no g54's. Otherwise I have a program that always stays in the control WPC, touch senser, manual program. Manual program is a center drill (can be anything) that rapids to X0.Y0., then to Z+3., finaly G00. I then go to work offset page and teach the coords in

[greybeard]

Well, all the info was a help-but jack hit it right on for what I was looking for. The program ran the first time out-1 tweak on final size and away we went. Now that door is open I am looking at doing alot of my jobs differently. we have had the 1 seat for a couple of years now-nobody uses-what a shame. Well, that stops now-thank you.