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:

probe crash

swanny

By swanny,
in Industrial Forum

 Share

Recommended Posts

swanny Newbie

swanny

Posted
Posted

This has been the format for the probing cycle before we run a part. Its added to the front of a program so every part gets probed. The problem I just found was you cant start the program mid cycle because of the G91 Z- move. But as long as you run the program from the home position, it works fine. Need help to rewrite so I can start probe from anywhere in the program.

 

T24 M6

G90 G54 G0 X0 Y0

G91 Z- ( INSERT Z POSITION FROM HOME)

G65 P9995 W54 A11. D0.27 E-0.7

 

 

 

The other thing is the height offset for the probe is a set number. 5.5169 which is from the spindle to the tip of the probe.

Just need to be steered in the right direction.

Link to comment
Share on other sites
swanny Newbie

swanny

Posted
  • Author
Posted

Not really. What I'm trying to do is have a z offset for my probe. So it references a workoffset for a z movement instead of assuming its at the home position and incrementally moving down. I crashed a probe because of this. Anyone know if I can just give it a different length offset not being used. So for instance my probe is tool #24:

 

T24 M6

G90 G54 G0 X0 Y0 

G43 H34 Z5. 

G65 P9995 W54 A11. D0.27 E-0.7

Link to comment
Share on other sites
Mick Contributor

Mick

Posted
Posted

I encountered something similar a while back on our Okuma MU500. It seems the Okuma probe macro cancels any offset applied, and moves incrementally from the home position. I wanted to position the probe using the length offset/work offset, and then probe locally.

 

From memory, I had to revert back to the base macro and programme my own probe sequence.

Link to comment
Share on other sites
swanny Newbie

swanny

Posted
  • Author
Posted

I encountered something similar a while back on our Okuma MU500. It seems the Okuma probe macro cancels any offset applied, and moves incrementally from the home position. I wanted to position the probe using the length offset/work offset, and then probe locally.

 

From memory, I had to revert back to the base macro and programme my own probe sequence.

These movements are before the actual probing cycle starts though. Im going to test it out and see if this will work. I still want my probing cycle to work the same, Im just trying to give my probe a hard location to start from.

Link to comment
Share on other sites
AMCNitro Enthusiast

AMCNitro

Posted
Posted

Im assuming this is on a Haas, do you also have the tool offset probe?  If I remember correctly( I didnt do a lot of this) the Z is programmed from the machine home position. 

Also, theres a PDF that you can get from one of the Haas reps that shows you all kinds of things that can be done with the probe, my last job had it, I just never got a chance to really look at it.

Link to comment
Share on other sites
jlw™ Newbie

jlw™

Posted
Posted

Sounds like you need to find the parameter and turn off motion on G43/G49 to me. I would only use the protected positioning cycles.

 

Your first sample did not have G43 but the second does. Did that not fix it?

 

I've also seen where if you don't call the probe tool change (even if it's in the spindle) you don't get the G43 length offset properly.

 

What control is this on?

Link to comment
Share on other sites
taperlength Newbie

taperlength

Posted
Posted

Not really. What I'm trying to do is have a z offset for my probe. So it references a workoffset for a z movement instead of assuming its at the home position and incrementally moving down. I crashed a probe because of this. Anyone know if I can just give it a different length offset not being used. So for instance my probe is tool #24:

 

T24 M6

G90 G54 G0 X0 Y0 

G43 H34 Z5. 

G65 P9995 W54 A11. D0.27 E-0.7

 

If your machine is like the one I have been using,  the probe uses a parameter setting for calculating probing in Z, which should be the same as the Z tool offset.

You should be able to use any offset number but might want to have a line that sets it just in case it got changed.

 

G10 L10 P34 R5.5169   (sets tool offset 34 to 5.5169)

 

Also put in a G91 G28 Z0  before the G90 G54 X0 Y0  so in case it does not actually do a tool change, it won't crash into something.

 

When ever the probe is close to the part, it should be positioned using a protected move.  On a Haas it would be G65 P9810, on other machines it might be G65 P9510 or something else.

Link to comment
Share on other sites
Sticky Newbie

Sticky

Posted
Posted

Are you running Inspection Plus?

 

You should have a tool length offset active for your probe. You should be able to use G43 for your probe like any other tool. After your programmed Z command to activate the tool length offset, use 9810 for protected positioning.

 

ie:

 

M6 T151 (PROBE)
T1 (FACEMILL)
G0 G90 G54 X0 Y0
M59 (PROBE ORIENT ON)
G43 H151 Z2.
G65 P9810 F50. Z.2 (PROTECTED POSITIONING TO FEED PLANE)
G65 P9811 Z0. T1. (CALIBRATE FACEMILL TOOL LENGTH)
G65 P9810 Z2. (PROTECTED POSITIONING TO RAPID PLANE)
M58 (PROBE ORIENT OFF)
G91 G28 X0. Y0. Z0.
M6 T1
G90
M30

 

Why are you using G91?

Link to comment
Share on other sites
swanny Newbie

swanny

Posted
  • Author
Posted

Are you running Inspection Plus?

 

You should have a tool length offset active for your probe. You should be able to use G43 for your probe like any other tool. After your programmed Z command to activate the tool length offset, use 9810 for protected positioning.

 

ie:

 

M6 T151 (PROBE)

T1 (FACEMILL)

G0 G90 G54 X0 Y0

M59 (PROBE ORIENT ON)

G43 H151 Z2.

G65 P9810 F50. Z.2 (PROTECTED POSITIONING TO FEED PLANE)

G65 P9811 Z0. T1. (CALIBRATE FACEMILL TOOL LENGTH)

G65 P9810 Z2. (PROTECTED POSITIONING TO RAPID PLANE)

M58 (PROBE ORIENT OFF)

G91 G28 X0. Y0. Z0.

M6 T1

G90

M30

 

Why are you using G91?

Thats just it. I dont want to use a G91. This is what I was told how it was setup before. I dont like it. This is a haas control on a VF-2 SS. Yes it is inspection plus. The machined part is on a small fixture. The part has a really tight true position tolerance on it. So the probe comes down and touches off on the part each time, sets a new offset, then runs the machining process. They normally use the machine home location for  a z location and, eyeball the probe to a starting point and then edit that in the program as an incremental move from the home position. works great until you arent in the home position, then it crashes.

Link to comment
Share on other sites
Sticky Newbie

Sticky

Posted
Posted

Thats just it. I dont want to use a G91. This is what I was told how it was setup before. I dont like it. This is a haas control on a VF-2 SS. Yes it is inspection plus. The machined part is on a small fixture. The part has a really tight true position tolerance on it. So the probe comes down and touches off on the part each time, sets a new offset, then runs the machining process. They normally use the machine home location for  a z location and, eyeball the probe to a starting point and then edit that in the program as an incremental move from the home position. works great until you arent in the home position, then it crashes.

 

Wow. The guy before you that set that up didn't understand what he was doing at all.

 

Make sure you have the right length for your probe in your tool length offset page, and do what I showed above. You can program your probe to use local work offsets and tool lengths just like any other tool.

 

Have you re calibrated your probe since you crashed it?

  • Like 1
Link to comment
Share on other sites
Tim Johnson Enthusiast

Tim Johnson

Posted
Posted

Here's my probe calibration program (for Fanuc)

%
O7001(PROBE TOTAL CALIBRATION)
(K:NCSYS\ENSHU GE480H\PROBE\AUTO-CAL192.NC)
 
(THIS WILL USE THE AUTO-CALIBRATION FIXTURE)
(FIXTURE OFFSET -- G54)
(XOYO CENTERLINE -- Z TOP OF RING GAGE)

M00(SET STYLUS LENGTH WITH A TAPE MEASURE)
(THIS PROGRAM MUST BE RUN ON PALLET A)
 
#5221=0
#5222=0
#5223=#921
#5224=0
G00 G17 G20 G40 G49 G80 G90 G94
M06 T04 (4" LONG PROBE)
G10L52
N6202R00000001
G11
M19

G54 X3.1 Y-31.5
G43 H04 Z13.
G65 P9810 Z11.3 F20.
G65 P9801 Z10.8425 T04
G65 P9810 Z13. F200.
G65 P9810 X.00317 Y-30.63638
G65 P9810 Z10.7
G65 P9802 D1.
G65 P9804 D1.
G65 P9810 Z13. F200.
M30
%

#921 is the distance from G28  Z home to the center of the pallet. We also use a calibration plate that attaches to pallet 1 and every machine has their own program.

Link to comment
Share on other sites
swanny Newbie

swanny

Posted
  • Author
Posted

Here's my probe calibration program (for Fanuc)

%
O7001(PROBE TOTAL CALIBRATION)
(K:NCSYS\ENSHU GE480H\PROBE\AUTO-CAL192.NC)
 
(THIS WILL USE THE AUTO-CALIBRATION FIXTURE)
(FIXTURE OFFSET -- G54)
(XOYO CENTERLINE -- Z TOP OF RING GAGE)

M00(SET STYLUS LENGTH WITH A TAPE MEASURE)
(THIS PROGRAM MUST BE RUN ON PALLET A)
 
#5221=0
#5222=0
#5223=#921
#5224=0
G00 G17 G20 G40 G49 G80 G90 G94
M06 T04 (4" LONG PROBE)
G10L52
N6202R00000001
G11
M19

G54 X3.1 Y-31.5
G43 H04 Z13.
G65 P9810 Z11.3 F20.
G65 P9801 Z10.8425 T04
G65 P9810 Z13. F200.
G65 P9810 X.00317 Y-30.63638
G65 P9810 Z10.7
G65 P9802 D1.
G65 P9804 D1.
G65 P9810 Z13. F200.
M30
%

#921 is the distance from G28  Z home to the center of the pallet. We also use a calibration plate that attaches to pallet 1 and every machine has their own program.

Thanks for your help. Works great

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...