Mastercam posts on Mazak

[60rock]

I am having problems getting the EIA program I created to read the Matatrol tool data page. Problems are occuring in both length and Diameter comps. The tools do not cut at same height as programmed. This could also be due to the use of both having a probe and automatic tool height measurement system both, of which, are broken. Lastly teaching the Z axis coordinate on the EIA side using G54 does not match what I get on a mazatrol work coordinate unit.

Any help would be great. Hopefully I can return the favor to someone.

[mbi]

First what control do you have?
I use Eia on our m-32. First you must decide if you are going to program from the center of the cutter or the peripheral of the cutter. I use the center of the cutter and use cutter comp.
You must set your parameters to read cutter comp. I am at home until Monday and don't have the info handy however it is in your E95 parameter I think?
Your Mazak will read your tool data page for tool length I think. Check your book to be sure. All our Mazaks use Mazatrol tool Data for tool length.
You must set all your tool offsets to 0 to control your cutter comp.
For example:
Tool # 1 is a 1.0 diameter end mill that is reground to .990. You will put your end mill into pocket #1 and go to you tool offset page and set tool offset comp #1 to -.005.
Use a D code next to your g41 or g42.
Teach your WPC’S to G54 and use g54 in your Eia code.
we also use a probe however you must use the inspection plus software to teach you g54.

I can't answer why teaching the Z axis coordinate on the EIA side using G54 does not match what I get on a mazatrol work coordinate unit. Our newer m32's to present mazaks you can run a probing unit in your mazatrol program using g54 in your additional wpc's on your wpc line.

[60rock]

The control in particular is a nexus 640. Thank you for the help on the cutter comp. for G41, that makes sense. the parameter settings were already altered and your parameter number is close to the one I had to change. I guess I was hoping that the G41 and G43 commands would match the mazatrol tool offset page in it's entirety.

For G43, I would use a H# according to the tool I want in the mazatrol tool data page?

For G41 I would enter a D# in the tool offset page(the one different than the main mazatrol tool offset page) and use the difference in the cutter diameter as the inputted value. Do I have this correct?

What, exactly, is the inspection plus software and it's capabilities? I will try to look it up online as well.

Right now both the automatic height measuring system and the probe are broken. In order to complete the part I made I needed to teach each tool off of the workpiece. Can I teach each tool of of a 3" block and back-figure a Z coordinate in order to eliminate teaching every tool off the work?

Thank you very much for your input.

[mbi]

You do not need an H with your g43. All you need is g43 and tool number. No H code. It should read the tool data page tool length. There is a parameter for this.

You are correct on the D code and g41. However check the parameter in your book so your machine knows to read the tool offset page not the tool data page for your tool offsets.

The inspection plus software is used to probe a plate in g code using macros.

[60rock]

Just to double check, the height offset line would look like

G43 T1

if using tool 1?

[psychomill]

No.. You do a tool call as normal then for a G43 line, you don't need to specify an H number...

T1M6
.
.
G43Z.1 (no H)


This is provided that your parameters and/or Tool Data page isn't telling the machine to look at the Offset page. If you're using the Offset page by iteself, then you need to use H as normal...

G43H1Z.1

[mbi]

This is a sample of the g43 and mazatrol tool data.

As psychomill said G43 Z 2.0 (no H)



O2552
(/////////////////////////////////)

(Job 2554 2 plate + setup 11-09-2009)

(\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\)

(Plate Size 4_STEEL )
(X 35.5 )
(Y 17.875 )
(Z 3 )


(********************************)
(WPC X = -28.209 )
(WPC Y = -25.0975 )
(WPC Z = -33.567 )
(********************************)

( T97 = EM.75 C CARBIDE )
N10 G0 G40 G64 G80 G94
N12 G30 G91 Z0.
N14 G30 Y0.
N16 T97
N18 M6
N20 G0 G17 G54 G90 X-5.0145Y-9.5171 M38 S 750 M3
N22 ( T97 DIA.=0.75 NAME=EM.75 C CARBIDE )
N24 ( FINISH SIDE MILL_WIRE_SLOT_2_150_DEEP )
N26 M1
N28 M8
N30 G43 Z2.0 T97
Z-1.55
G1 Z-2.158 F150.0
G41 D97G62 X-4.8593 Y-8.9375 F10.0
Y-5.7814
G3 X-4.9343 Y-5.7064 I-0.075 J0. F7.0
G1 X-5.0343 F10.0
G3 X-5.1093 Y-5.7814 I0. J-0.075 F7.0
G1 Y-8.9375 F10.0
G40
X-4.954 Y-9.5171
X-5.0145
G41 D97G62 X-4.8593 Y-8.9375
Y-5.7814
G3 X-4.9343 Y-5.7064 I-0.075 J0. F7.0
G1 X-5.0343 F10.0
G3 X-5.1093 Y-5.7814 I0. J-0.075 F7.0
G1 Y-8.9375 F10.0
G40
X-4.954 Y-9.5171
G0 Z2.0
N72 ( PROGRAM END )
N74 M9
N76 G0 G28 G91 Z0 M5
N78 G28 G91 Y0
N80 G0 G90 G53 X-10.0
N82 G90 M30

[mbi]

Did you change par F93 bit 4? It should look like this 00101000. This Par enables the EIA to read the Matatrol tool data page tool length.

Just another thought? Is your post outputting code from the tool center or the peripheral? You will need it to output from the tool center. In my cam software I can program from either.

[60rock]

I changed that parameter, as well as another one that deals with tool height.

How does your software differentiate between the tool center or peripheral?

[mbi]

It is just a flag I check if I want to part line program or tool center line program.