Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Laser tool setter macro for wear comp

Thad

By Thad,
in Industrial Forum

 Share

Recommended Posts

Thad Enthusiast

Thad

Posted
Posted

When I started at this company last month, everyone was using control comp. I got them switched over to wear, but the way the laser tool setter works, from my understanding, is that it detects the tool diameter, divides it in 2, then enters that value into the tool offset page. That works fine for control comp but I need it to figure the wear value. From what the operator tells me, he can't even look at the code for this macro, let alone edit it. Do we need a new macro to do this? How is this done? Currently, the operators are hand editing the wear value in.

 

Here is the info that I have been given. I'm not familiar with any of it so if you need more info, let me know and I'll ask. Any help would be greatly appreciated.

 

Machine:

Mazak

Nexus 410A

Model# VCN-410A

 

Control:

Mazatrol

PC-Fushion-CNC 640M

 

Laser:

Renishaw NC1 F200

 

 

Thad

Link to comment
Share on other sites
Thad Enthusiast

Thad

Posted
  • Author
Posted

quote:
If ya want I can send the NC-1 books in pdf format.

Jimmy, I found this manual at Renishaw's site: "NC1 non-contact tool setting system Programming Guide (Fanuc compatible)" I'm currently looking through it. If you have any other info, feel free to send it.

 

quote:
Oh,btw if ya unlock the 9000 series programs for editing you can look at those programs I believe.

Do you now how to unlock those?

 

 

B, I'll look into the F paramters.

 

Thad

Link to comment
Share on other sites
Thad Enthusiast

Thad

Posted
  • Author
Posted

quote:
here's the line you need to find in the macro

#109=1(OFFSET-RADIUS 1/DIAMETER 2)

Maybe I'm wrong on this, but it looks like that just tells the laser whether to find the dia or radius of the tool. With wear comp, I need the difference between the programmed size and the actual size. For example, if I programmed for a .500 cutter, but the tool we're actually using is a resharp and measures .490, I need a value of -.005 (the machine takes radius offsets) entered into the offset table. Does that make sense? Somehow, the tool setter needs to know the programmed tool size in order to calculate the difference.

 

Thad

Link to comment
Share on other sites
robk Newbie

robk

Posted
Posted

Here is a longer sample @ the beginning of the program...

We could skip it by having block delete 8 active.

Make sure that you don't use block delete 2 with the program, because then you would have to put your division formula in brackets.

 

 

()

()

()

()

(SET TLO AND WEAR FOR ALL TOOLS EXCEPT THE RIGHT ANGLE HEAD)

()

()

/8T24 T25 M06

/8G65 P9862 B3. T24 D24 I.375 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T25 M06 T26

/8G65 P9862 B3. T25 D25 I.375 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T26 M06 T27

/8G65 P9862 B3. T26 D26 I.375 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T27 M06 T28

/8G65 P9862 B1. T27 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T28 M06 T29

/8G65 P9862 B3. T28 D28 I.625 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T29 M06 T30

/8G65 P9862 B3. T29 D29 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T30 M06 T31

/8G65 P9862 B3. T30 D30 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T31 M06 T32

/8G65 P9862 B3. T31 D31 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T32 M06 T33

/8G65 P9862 B3. T32 D32 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T33 M06 T34

/8G65 P9862 B3. T33 D33 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T34 M06 T35

/8G65 P9862 B3. T34 D34 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T35 M06 T36

/8G65 P9862 B3. T35 D35 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T36 M06 T37

/8G65 P9862 B3. T36 D36 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T37 M06 T38

/8G65 P9862 B3. T37 D37 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T38 M06 T39

/8G65 P9862 B3. T38 D38 I.250 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T39 M06 T40

/8G65 P9862 B3. T39 D39 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T40 M06 T42

/8G65 P9862 B3. T40 D40 I.500 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T42 M06 T43

/8G65 P9862 B3. T42 D42 I.625 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T43 M06 T44

/8G65 P9862 B1. T43 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T44 M06 T45

/8G65 P9862 B1. T44 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T45 M06 T46

/8G65 P9862 B3. T45 D45 I4.00 /2S1000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T46 M06 T47

/8G65 P9862 B3. T46 D46 I4.00 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T47 M06 T48

/8G65 P9862 B3. T47 D47 I4.00 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T48 M06 T49

/8G65 P9862 B1. T48 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T49 M06 T50

/8G65 P9862 B1. T49 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T50 M06 T51

/8G65 P9862 B3. T50 D50 I.250 /2S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T51 M06 T52

/8G65 P9862 B1. T51 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T52 M06 T53

/8G65 P9862 B1. T52 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T53 M06 T54

/8G65 P9862 B1. T53 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T54 M06 T58

/8G65 P9862 B1. T54 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

/8T58 M06 T24

/8G65 P9862 B1. T58 S3000

/8G91 G28 X0. Y0. Z0. B0. C0.

()

()

()

Link to comment
Share on other sites
YoDoug® Newbie

YoDoug®

Posted
Posted

We have contact tool setters but this is from the Renishaw manual. Enter an I value in your g65 call for the nominal size of the cutter.

 

Ii i = Size adjustment to compensate

for cutting conditions. A positive

value sets the tool radius small by

the stated amount, e.g. I=.01 sets

the cutter radius small by 0.01.

Link to comment
Share on other sites
Thad Enthusiast

Thad

Posted
  • Author
Posted

Rob and Doug,

 

I'm not familiar with what the code is even supposed to look like. Say I was going to write a program that would only set the tool length and wear dia of tool 5 that is programmed for .500? Would it look like this?

 

code:
T5 M06

G65 P9862 B3. T5 D5 I.500 /2S3000

G91 G28 X0. Y0. Z0. B0. C0.

I used your example from above. Is the G91 line needed? What is the B in the second line? All I want it to do is set the tool length/dia and then end the program.

 

Thad

Link to comment
Share on other sites
robk Newbie

robk

Posted
Posted

The G91 line is not really needed. I'm just sending the tool to it's home position (better safe then sorry).

B1.= Set The Length

B2.= Measure The Dia.

B3.= Measure The Length & Dia.

 

T5. is the offset # (not tool #)... So even though you have Tool #5 In the spindle you could tell it to put the offset into a different #.

 

D5. is same as above, but for dia. offset #

 

I.5 Is the Dia. Of Your Tool

 

/2 just divides that dia. by 2 (which is the info you're looking for)

 

S is your spindle speed

Link to comment
Share on other sites
Thad Enthusiast

Thad

Posted
  • Author
Posted

Is there a way to put a name or description in the program? I'm used to seeing whatever is after the "(" or "*" on the first line to be the program name and be displayed like this in the control...

 

O1234 (MILL POCKET)

 

Can that be done on this control? I can name the program (MILL POCKET) once it's in the control, but I would like it to be read in with the file.

 

Thad

Link to comment
Share on other sites
  • 2 years later...
Thad Enthusiast

Thad

Posted
  • Author
Posted

Another question on the laser tool setter...

 

All of our taps are T7, but they each have a different H value. Is there a way to assign how the laser values are stored? Right now, if T7 is being measured, it gets stored in H7. I'd like to tell it T7 goes with H33 when I'm measuring a 1/4 tap, T7 goes with H34 when I'm measuring a 5/16 tap, etc.

 

Perhaps something along these lines to set H33...

 

code:
T7 H33 M221

or H34...

 

code:
T7 H34 M221

Am I explaining this well enough?

 

Thad

Link to comment
Share on other sites
Ron Branch @ Verisurf Newbie

Ron Branch @ Verisurf

Posted
Posted

Well when you do this it stores the information to a variable on the machine. You should be able to access that variable. From that you would want to write a logic that would take the H7 value and then store it in the h33 value. Should be pretty straight forward a process to do. You could get fancy and have the post make the macro for you, but really up to you how much work you want to put into it.

 

HTH

Link to comment
Share on other sites
robk Newbie

robk

Posted
Posted

Hey Thad, this is from above

 

quote:
T5. is the offset # (not tool #)... So even though you have Tool #5 In the spindle you could tell it to put the offset into a different #.

If you parameters are set correctly you should just change the T value to the offset#, or as Ron suggested you could use some logic to force the values in.

Shoot me an e-mail if you want a copy of the variables that correspond to your tool offsets.

 

 

BTW, it was a pleasure to meet you Ron @ Eastec smile.gif

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...