What's new
What's new
By:
Advanced search…

Haas Renishaw Probing Issues

T

Taylor-WSE

Plastic
Joined
Apr 24, 2019
I'm missing something here and need some help.

All I'm trying to do is set a work offset by probing a bore. I have no problem setting an offset when I'm doing single-surface probing cycles but for some reason I'm struggling with the bore cycle. I believe my code below is correct but the machine just refuses to update the G54 X&Y offsets. I have verified macro variables 185 & 186 (X&Y position taken from P9814 cycle) are correct, they just aren't updating the work offset.

This is on a next gen control Haas VF. I'm writing the program instead of using VPS because long term I'm going to have the program level an A-Axis rotary.

My ideas...
  • Next gen 9000 programs are structured differently than classic control?
  • Syntax error, maybe a decimal etc.?

Please let me know if you need any more information and thank you in advance for any input.

Code: 
O101 (Set WCS Off Bore)
(Jog probe into place)
G54
G90
G43 H31
G103 P1
G65 P9832 (Probe On)
G65 P9814 D1.5 S1 (Probe trunnion bore)
G65 P9833 (Probe Off)
M30
 
Taylor-WSE said:
I'm missing something here and need some help.

All I'm trying to do is set a work offset by probing a bore. I have no problem setting an offset when I'm doing single-surface probing cycles but for some reason I'm struggling with the bore cycle. I believe my code below is correct but the machine just refuses to update the G54 X&Y offsets. I have verified macro variables 185 & 186 (X&Y position taken from P9814 cycle) are correct, they just aren't updating the work offset.

This is on a next gen control Haas VF. I'm writing the program instead of using VPS because long term I'm going to have the program level an A-Axis rotary.

My ideas...
  • Next gen 9000 programs are structured differently than classic control?
  • Syntax error, maybe a decimal etc.?

Please let me know if you need any more information and thank you in advance for any input.

Code: 
O101 (Set WCS Off Bore)
(Jog probe into place)
G54
G90
G43 H31
G103 P1
G65 P9832 (Probe On)
G65 P9814 D1.5 S1 (Probe trunnion bore)
G65 P9833 (Probe Off)
M30
Click to expand...

I dont know G103

but you dont have a X0Y0 call after you instate work offset G54

You are doing a "referred zero" routine here because of that. To make that work you have to have rough origin, activate it and position the probe into the reference feature with position calls relating to that desired origin.

iE, The center of the bore is XY zero

G90
G54
G65P9810 X0. Y0. F150. (protected pos)
G65P9814 D1.5 S1.

ie, the center of the bore is at X-100 y-100

G90
G54
G65P9810 X-100. Y-100. F150. (protected pos)
G65P9814 D1.5 S1. (sets G54 x+100 y+100 from the center of this bore)

the WIPS routine same as GOPROBE handle this automatically while you are setting up. So you don't realize that its needed in a program.
 
Taylor-WSE said:
I'm missing something here and need some help.

All I'm trying to do is set a work offset by probing a bore. I have no problem setting an offset when I'm doing single-surface probing cycles but for some reason I'm struggling with the bore cycle. I believe my code below is correct but the machine just refuses to update the G54 X&Y offsets. I have verified macro variables 185 & 186 (X&Y position taken from P9814 cycle) are correct, they just aren't updating the work offset.

This is on a next gen control Haas VF. I'm writing the program instead of using VPS because long term I'm going to have the program level an A-Axis rotary.

My ideas...
  • Next gen 9000 programs are structured differently than classic control?
  • Syntax error, maybe a decimal etc.?

Please let me know if you need any more information and thank you in advance for any input.

Code: 
O101 (Set WCS Off Bore)
(Jog probe into place)
G54
G90
G43 H31
G103 P1
G65 P9832 (Probe On)
G65 P9814 D1.5 S1 (Probe trunnion bore)
G65 P9833 (Probe Off)
M30
Click to expand...

Inspection + philosophy is, that it is not setting the desired WCS in the center of measured feature, but is updating the existing coordinates of the WCS by the deviation between coordinates of starting point and found center of the measured feature. It means, that in order to set the WCS in the center of arbitrary bore, you have to bring the probe to its approximate center, set the WCS there and then execute the measurement. If you know approximate position of the bore in current WCS, command it to move to center of the bore, otherwise bring it manually. Let’s assume, that your current WCS is G54, in which your bore coordinates are X-100., Y-100., and you wish to set the G55 in the center of the bore. The program, assuming that Z surface is 0 in G54, and probe tool number is XX :
G90
M6 TXX
G54
G43 HXX Z[#5043-#[11000+XX]] F10 (apply tool offset without move in Z)
G65P9810 X-100. Y-100. F150. (protected move to center of the bore)
G6Z P9810 Z-.5 F150. (protected move into the bore)
#5241=#5021 (set current X position as G55 X WCS)
#5242=#5022 (set current Y position as G55 Y WCS)
G55
G65P9814 D1.5 S2. (updates G55 X an Y WCS to the center of bore)

Pay attention, that #185 and #186 show the coordinates of the center of just measured bore in CURRENT work coordinates system.
 
Alrighty I've played around with it a little bit more and I'm going to take bits and pieces from each reply.

GENERALDISARRAY: G103 sets the block look-ahead, I've seen it recommended from multiple sources when you are working with subs. Might be unnecessary but hasn't caused any issues for me so far. Thank you for the explanation, it helps out a lot.

PROBE: Your explanation also helped out a lot but setting the current position to a WCS was the part I needed. My goal for this program was to jog the probe to a bore, then hit cycle start so this works perfectly.

LARRY: I didn't see any change between having the decimal on the S parameter or not, though that one has bit me on other programs... I agree the most elegant way of doing it is to use the 9023 sub. My main reason(s) for avoiding it was to save on cycle time (turning probe on and off between protected moves) and to get the programming looking similar to what our CAM software (fusion 360) spits out when doing probing cycles. But I suppose for setups cycle time isn't going to kill me.

Thanks for the advice guys. Final(ish) code below.

Code: 
G90 G54
(jog probe in place)
(set current position to G54)
#5221 = #5021
#5222 = #5022
(protected move to G54 X0 Y0)
G43 H31
G65 P9832 (ON)
G54 G65 P9810 X0. Y0. F10. (POS)
(probe bore)
G65 P9814 D1.5 S1 (BORE)
G65 P9833 (OFF)
M30
 
You must log in or register to reply here.

Similar threads

S
PROBE BOSS TO SLOT TROUBLESHOOTING
Replies
4
Views
501
hi-fly-cnc
H
russmill
Strange Renishaw OMP-40-2 probe open issue
Replies
5
Views
569
russmill
russmill
J
Renishaw Probe startup failure 1101
Replies
2
Views
2K
SpeedsandFeeds
S
V
In Process Probing
Replies
6
Views
720
VCI1759
V
M
Haas Probe Calibration Issue
Replies
5
Views
952
sinha
S








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top