Bill H

Probing Routine - Renishaw/Haas

Recommended Posts

2 minutes ago, Colin Gilchrist said:

Ron just posted some links to previous threads here where we've talked about Productivity Plus. 

It is a nice add-in to Mastercam, if you do a lot of Probing, and/or, you want to build custom Probing cycles, and use the Prod+  interface to write custom macro logic and add Sequence Blocks for program jumps (based on Probe results).

 

Yes I'm just going thru his links... To tell you the truth I'm even more confused ... LOL  Also at work we have a designated programmer  and he uses MC . No idea if his software has anything for custom probing cycles. What I'm doing at work is kind of all on my  own with no support. We have a 2013 Haas VF4 with probe and setter. No one ever uses it and I've been the soul person running it for almost a year now. I think once I can get some of this figured and understand it, I may be able to find lots of places to use the probe other than work offsets.

Share this post


Link to post
Share on other sites
17 minutes ago, FLR169 said:

Yes I'm just going thru his links... To tell you the truth I'm even more confused ... LOL  Also at work we have a designated programmer  and he uses MC . No idea if his software has anything for custom probing cycles. What I'm doing at work is kind of all on my  own with no support. We have a 2013 Haas VF4 with probe and setter. No one ever uses it and I've been the soul person running it for almost a year now. I think once I can get some of this figured and understand it, I may be able to find lots of places to use the probe other than work offsets.

Ok, then really, you need to start at the very beginning. 

https://www.haascnc.com/content/dam/haascnc/en/service/reference/probe/renishaw-inspection-plus-programming-manual---2008.pdf

Start with reading the Probing Manual for that machine, which is what that link will take you to. 

The Probe gets installed on the Haas with a bunch of programs from the factory to perform different measurements. Yes, you can use the 'automated routines' on the Haas control to call some of the programs, but to harness the true power of that Probe, you need to understand the main macro programs, and how to 'pass parameters' to the Macro Call line. (G65 P9810 is a macro call, so is G65 P9814) the Alpha Addresses that follow the Macro Call are letters. (The value of each Letter is passed internally to the Macro Program, as a 'Local Variable' (#1-#33).

Typically, you are setting Work Offsets or Measuring Features with the Spindle Probe. You set Tool Length Offsets (H Values), with the Tool Touch Probe.

 

  • Like 1

Share this post


Link to post
Share on other sites

Also, read this in your spare time:

https://www.haascnc.com/content/dam/haascnc/en/service/manual/operator/english---mill-operator's-manual---2014.pdf

(Try putting in an hour in the evenings before bed of light reading.) 🙂

https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/mill---programming-workbook.pdf

You mentioned that you are not the one programming the machine. Depending on how much knowledge you have of being a Machine Operator, versus Programming knowledge, the Mill Workbook is also a good place to start. The workbook has machining and programming theory and knowledge, where the Operator's Manual kind of already assumes that you know how to program G-Code.

Share this post


Link to post
Share on other sites

One key thing one needs to understand about Productivity Plus is it is skip signal based and not cycle based. Meaning you program a 4 point bore in Prod. Plus, you're not going to get a position to the center of the bore then the G65P9814... bore cycle. You're going to 4 individual measurement points and a bunch of protected moves in between. Then if you wanted to get the #135-#149 variable data based on the cycle, you won't have that data available.

Food for thought.

Share this post


Link to post
Share on other sites
9 hours ago, Colin Gilchrist said:

Also, read this in your spare time:

https://www.haascnc.com/content/dam/haascnc/en/service/manual/operator/english---mill-operator's-manual---2014.pdf

(Try putting in an hour in the evenings before bed of light reading.) 🙂

https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/mill---programming-workbook.pdf

You mentioned that you are not the one programming the machine. Depending on how much knowledge you have of being a Machine Operator, versus Programming knowledge, the Mill Workbook is also a good place to start. The workbook has machining and programming theory and knowledge, where the Operator's Manual kind of already assumes that you know how to program G-Code.

Morning 

I'm totally familiar with g-code and can program

We are a union shop...

Machinists in one programmer in the other one...(

No one  wants this tech to be used for the better.

It's been sitting in the drawer for a year +.

I'm very intrigued and interested in learning this.

I do have the inspection plus pdf printed off.

I'm very comfortable on our Haas . I'm sure there is stuff still to learn but i'll deal with that when needed

Also been machining 25 yrs and i mess around doing side jobs with Fusion 360.

So I have a good understanding 

Obviously not as good as you all...;)

Share this post


Link to post
Share on other sites
1 hour ago, FLR169 said:

Morning 

I'm totally familiar with g-code and can program

We are a union shop...

Machinists in one programmer in the other one...(

No one  wants this tech to be used for the better.

It's been sitting in the drawer for a year +.

I'm very intrigued and interested in learning this.

I do have the inspection plus pdf printed off.

I'm very comfortable on our Haas . I'm sure there is stuff still to learn but i'll deal with that when needed

Also been machining 25 yrs and i mess around doing side jobs with Fusion 360.

So I have a good understanding 

Obviously not as good as you all...;)

I didn't mean my post as a slight against your skills, but just making sure you have all the information I can possibly help provide.

Knowledge is Power.

I have worked in several Union shops, and completely understand the mentality you are fighting. Nobody wants to rock the boat, or stop the gravy train. Why do a task in 5 minutes, when you can take a good hour?

Since you're already familiar with the machine and programming, check out Mark Terryberry and the Haas channel on YouTube. You'll find a lot of good tips, tricks, and demonstrations, especially on using the Renishaw Probe.

 

 

Share this post


Link to post
Share on other sites
9 hours ago, cncappsjames said:

One key thing one needs to understand about Productivity Plus is it is skip signal based and not cycle based. Meaning you program a 4 point bore in Prod. Plus, you're not going to get a position to the center of the bore then the G65P9814... bore cycle. You're going to 4 individual measurement points and a bunch of protected moves in between. Then if you wanted to get the #135-#149 variable data based on the cycle, you won't have that data available.

Food for thought.

I don't believe that is 100% correct James.

I've configured the RenMF Files to output the existing Probe Cycles (9810, 9811, 9812, 9814), and was able to write Macro Logic directly in the Prod+ interface, to capture and save-off the #138-#149 Cycle Result Data.

The issue is that you have to enable a switch in the RenMF File, so that it only outputs the 'Cycle Calls', and does not print the full Probing Cycle Macros below the initial calls.

But you can absolutely configure the Prod+ Add-on to use the existing Inspection Plus cycles that are installed on the Haas. (or any other machine with a Renishaw Probe, where you want to use existing cycles on the machines.)

The only caveat and danger is if you have a mix of machines in the same shop, which have different configurations for the probing systems. In these cases, you can't just swap programs from machine-to-machine, and it would be better to have the Macro Programs printed at the bottom of the NC File, or as Separate Subroutine Files, if you need that "portability".

  • Like 1

Share this post


Link to post
Share on other sites

 

On 2/9/2021 at 5:50 PM, FLR169 said:

Great information here.  Can anyone shed a direction to figure out how to probe 4 corners and have the lowest corner inputted into my desired Z work offset'

Thanks Mike

You can try something like this;

G0 X1. Y-1. G59

G65 P9810 Z.91 F200.

G65 P9811 Z.41

G65 P9810 Z5.22

#150=#2706 <<<<<<<<<<<<<<<<<<<<<<

G0 X3.

G65 P9810 Z.91 F200.

G65 P9811 Z.41

G65 P9810 Z5.22

#151=#2706 <<<<<<<<<<<<<<<<<<<<<<<<<<

IF[#151LT#150]THEN#151=#150 <<<<<<<<<<<<

G0 Y-2.

G65 P9810 Z.91 F200.

G65 P9811 Z.41

G65 P9810 Z5.22

#151=#2706 <<<<<<<<<<<<<<<<<<<<<<

IF[#151LT#150]THEN#151=#150 <<<<<<<<<<<<<<<<<<<<

G0 X1.

G65 P9810 Z.91 F200.

G65 P9811 Z.41

G65 P9810 Z5.22

#151=#2706 <<<<<<<<<<<<<<<<<<<<<<<<<<<

IF[#151LT#150]THEN#151=#150 <<<<<<<<<<<<<

#2701=#2701+[#150-.01] <<<<<<<<<<<<<<<<<<<

M30

 

What you may need is something different but this should give you an idea on where to start.

 

image.png

  • Huh? 1

Share this post


Link to post
Share on other sites
7 minutes ago, crazy^millman said:

Tim how does that tap help? 🤣

I don't know how it got on. I deleted the attachment from my name even though I didn't put it there. I ordered  1/2 dozen of them yesterday.

Edit: Maybe it was still attached from me copying it and pasting into the e-mail but I copied the tool path so it should have disappeared.

  • Haha 2

Share this post


Link to post
Share on other sites
11 hours ago, Colin Gilchrist said:

I didn't mean my post as a slight against your skills, but just making sure you have all the information I can possibly help provide.

Knowledge is Power.

I have worked in several Union shops, and completely understand the mentality you are fighting. Nobody wants to rock the boat, or stop the gravy train. Why do a task in 5 minutes, when you can take a good hour?

Since you're already familiar with the machine and programming, check out Mark Terryberry and the Haas channel on YouTube. You'll find a lot of good tips, tricks, and demonstrations, especially on using the Renishaw Probe.

 

 

Hey Colin, I didn't take it that way...all good. Thought I should supply some info on me. I will do my best to go thru the inspection plus book. The Haas youtube channel is such a great service to us looking for answers via video. Always checking that page out.

  • Like 2

Share this post


Link to post
Share on other sites
On 2/9/2021 at 8:40 PM, cncappsjames said:

Like @Leon82 mentioned, the G65P9820 stock cycle could do it automatically. It's listed in the "Additional Cycles" section of your manual.

Hello,
   I heard about "G65 P9820", would you post out a complete code for this?

 

Thanks.

Share this post


Link to post
Share on other sites
On 4/21/2021 at 4:38 PM, SLuong said:

Hello,
   I heard about "G65 P9820", would you post out a complete code for this?

 

Thanks.

Did you look in the Manual?

Pages:

9-11, 9-12, 9-13, 9-14, & 9-15 > Explain it pretty well, with sample code!

https://www.haascnc.com/content/dam/haascnc/en/service/reference/probe/renishaw-inspection-plus-programming-manual---2008.pdf

It literally took me 3 seconds to find it.

CTRL + F

"P9820"

  • Thanks 1
  • Haha 2

Share this post


Link to post
Share on other sites
1 hour ago, Colin Gilchrist said:

Did you look in the Manual?

Pages:

9-11, 9-12, 9-13, 9-14, & 9-15 > Explain it pretty well, with sample code!

https://www.haascnc.com/content/dam/haascnc/en/service/reference/probe/renishaw-inspection-plus-programming-manual---2008.pdf

It literally took me 3 seconds to find it.

CTRL + F

"P9820"

I don't want to work I just want to lay in my hammock all day. :rofl:

  • Like 1

Share this post


Link to post
Share on other sites
2 hours ago, crazy^millman said:

I don't want to work I just want to lay in my hammock all day. :rofl:

I mean, I already posted a sample with explanation, on page 1 of the thread...

  • Like 1

Share this post


Link to post
Share on other sites
33 minutes ago, Colin Gilchrist said:

I mean, I already posted a sample with explanation, on page 1 of the thread...

Yes sir you did, but that is work and having to think for yourself. People want the easy button way of doing things where you just load the print in the front of the machine and the 800-1200 hours of programming is done and the 800-1200 run time is only 5 minutes and have a nice day. All that thinking and work is for crazy people like you and me. 😉 :hrhr: :thumbsup:

  • Like 1

Share this post


Link to post
Share on other sites
13 hours ago, crazy^millman said:

Yes sir you did, but that is work and having to think for yourself. People want the easy button way of doing things where you just load the print in the front of the machine and the 800-1200 hours of programming is done and the 800-1200 run time is only 5 minutes and have a nice day. All that thinking and work is for crazy people like you and me. 😉 :hrhr: :thumbsup:

https://youtu.be/XQ-9irXXIqI

Share this post


Link to post
Share on other sites
On 4/23/2021 at 12:06 PM, Colin Gilchrist said:

Did you look in the Manual?

Pages:

9-11, 9-12, 9-13, 9-14, & 9-15 > Explain it pretty well, with sample code!

https://www.haascnc.com/content/dam/haascnc/en/service/reference/probe/renishaw-inspection-plus-programming-manual---2008.pdf

It literally took me 3 seconds to find it.

CTRL + F

"P9820"

Hello Colin,
   I was able to do in HAAS and now I would like to do in MAZAK.  However, the sub program number as "P9820" of which STOCK ALLOWANCE you just old me was not found in MAZAK.  Do you where I can get a document of all the sub program call out for G65 as MAZAK?

 

ps: The control is fairly new, I think it is made in 2015 proximately. 

 

Thanks for the great info as HAAS

===================== this is what I've done for Haas ===============

O1234(PROBE TESTING)
N120(FIND LOWEST POINT ON SURFACE PROBE)
G0 G17 G40 G49 G80 G90
G91 G28 Z0.
T120 M6(RENAISHALL PROBE)
M0(CHECK G59 Z OFFSET VALUE)
(TAKE PICTURE OF IT)
G65 P9832(PROBE ON)      ==========> MISSING SUB- PROGRAM NUMBER FROM MAZAK
G0 G90 G59 X0. Y0.
G43 H#3020 Z1.
G1 Z.125 F25.
G65 P9820 Z0. I-4. J8.325 I4. J8.325 I-4. J.475 I4. J.475 S6.      ==========> MISSING SUB- PROGRAM NUMBER FROM MAZAK
G0 G90 Z1.
G91 G28 Z0.
M0(COMPARE G59 Z OFFSET FROM PREVIOUS VALUE)
(IT MUST BE DIFFERNT AT LEAST .0005 OR MORE)
M0(NOTHING CHANGE? DON'T RUN)
G65 P9833(PROBE OFF)      ==========> MISSING SUB- PROGRAM NUMBER FROM MAZAK
M30
%

Share this post


Link to post
Share on other sites
3 minutes ago, SLuong said:

  Do you where I can get a document of all the sub program call out for G65 as MAZAK?

Get a hold of your local Mazak Dealer and ask them to send them to you. Easy Peasy.

  • Thanks 1

Share this post


Link to post
Share on other sites
18 hours ago, SLuong said:

Hello Colin,
   I was able to do in HAAS and now I would like to do in MAZAK.  However, the sub program number as "P9820" of which STOCK ALLOWANCE you just old me was not found in MAZAK.  Do you where I can get a document of all the sub program call out for G65 as MAZAK?

 

ps: The control is fairly new, I think it is made in 2015 proximately. 

 

Thanks for the great info as HAAS

===================== this is what I've done for Haas ===============

O1234(PROBE TESTING)
N120(FIND LOWEST POINT ON SURFACE PROBE)
G0 G17 G40 G49 G80 G90
G91 G28 Z0.
T120 M6(RENAISHALL PROBE)
M0(CHECK G59 Z OFFSET VALUE)
(TAKE PICTURE OF IT)
G65 P9832(PROBE ON)      ==========> MISSING SUB- PROGRAM NUMBER FROM MAZAK
G0 G90 G59 X0. Y0.
G43 H#3020 Z1.
G1 Z.125 F25.
G65 P9820 Z0. I-4. J8.325 I4. J8.325 I-4. J.475 I4. J.475 S6.      ==========> MISSING SUB- PROGRAM NUMBER FROM MAZAK
G0 G90 Z1.
G91 G28 Z0.
M0(COMPARE G59 Z OFFSET FROM PREVIOUS VALUE)
(IT MUST BE DIFFERNT AT LEAST .0005 OR MORE)
M0(NOTHING CHANGE? DON'T RUN)
G65 P9833(PROBE OFF)      ==========> MISSING SUB- PROGRAM NUMBER FROM MAZAK
M30
%

Those Program Numbers are for a Renishaw Probe package. Contact Mazak to have them install a Renishaw set of Macros, so that you'll have access to the correct Macro Programs. 

Renishaw also makes 'Probing Packages with different capabilities'. So not every Macro Program may be present. In that case, you would need to contact Renishaw for an upgrade. 

  • Thanks 1

Share this post


Link to post
Share on other sites
On 4/26/2021 at 12:06 PM, crazy^millman said:

Get a hold of your local Mazak Dealer and ask them to send them to you. Easy Peasy.

@Colin Gilchrist  @crazy^millman

2013 Haas VF4 with probing and tool setter

So finally got the batteries needed for Probe and Tool Setter. I got it all setup and working. 

Today the weldment job showed up so I played around with the probing of the Z surface.

I had it probe the 4 corners in Z and input each corner to a Z work offset ( G55 thru G58 )

Then i picked my biggest Z # for my G54 work offset. ( This part done by me manually inputting the new Z #)

So I went thru this post and came up with this code to try tomorrow. ( also went thru the Inspection Plus  on P9820 )

G20 G40 G80 G17

G103 P1 (Block Look Ahead)

T25 M6 ( Probe )

G90 G0 G54 X.5 Y-.5

G43  z2.0 H25

G65 P9832 (Probe on)

G65 P9810 X.5 Y-.5 Z.25 F100. (Protected Move to P1)

G65 P9820 Z.25 I6. J-.5 I6. J-.5 I.5 J-5. S1 (P2 TO P4)

G65 P9833 (Probe off)

G0 G90 Z2.0

G91 G28 Z0

G103 ( Activate  Look Ahead )

M30

On the p9820 line I'm not sure what my Z should be.....the Z.25 will locate the probe .25 above the previous  Z0

Am I in the ball park with this.

Just so we are on the same page. After probing the 4 locations in Z, I want the biggest Z # to become my G54 Z work offset #.

Thanks for any input

Mike

Share this post


Link to post
Share on other sites
7 hours ago, FLR169 said:

G103 ( Activate  Look Ahead )

I may be wrong here but does the statement not have to read G103 P0 to cancel?

This is how it is for our DS30y. Although, in all honesty, I haven't tried it without the P0.

 

I hope this doesn't come across as too  condescending... seems to be a common theme lately.

4 minutes ago, AHarrison1 said:

I may be wrong here but does the statement not have to read G103 P0 to cancel?

This is how it is for our DS30y. Although, in all honesty, I haven't tried it without the P0.

 

I hope this doesn't come across as too  condescending... seems to be a common theme lately.

Nevermind, found the answer. It can be either/or

 

https://staging-diy.haascnc.com/g103-limit-block-look-ahead-group-00

Share this post


Link to post
Share on other sites
39 minutes ago, AHarrison1 said:

I may be wrong here but does the statement not have to read G103 P0 to cancel?

This is how it is for our DS30y. Although, in all honesty, I haven't tried it without the P0.

 

I hope this doesn't come across as too  condescending... seems to be a common theme lately.

Nevermind, found the answer. It can be either/or

 

https://staging-diy.haascnc.com/g103-limit-block-look-ahead-group-00

Morning 

Not condescending at all 

 

Share this post


Link to post
Share on other sites
10 hours ago, FLR169 said:

@Colin Gilchrist  @crazy^millman

2013 Haas VF4 with probing and tool setter

So finally got the batteries needed for Probe and Tool Setter. I got it all setup and working. 

Today the weldment job showed up so I played around with the probing of the Z surface.

I had it probe the 4 corners in Z and input each corner to a Z work offset ( G55 thru G58 )

Then i picked my biggest Z # for my G54 work offset. ( This part done by me manually inputting the new Z #)

So I went thru this post and came up with this code to try tomorrow. ( also went thru the Inspection Plus  on P9820 )

G20 G40 G80 G17

G103 P1 (Block Look Ahead)

T25 M6 ( Probe )

G90 G0 G54 X.5 Y-.5

G43  z2.0 H25

G65 P9832 (Probe on)

G65 P9810 X.5 Y-.5 Z.25 F100. (Protected Move to P1)

G65 P9820 Z.25 I6. J-.5 I6. J-.5 I.5 J-5. S1 (P2 TO P4)

G65 P9833 (Probe off)

G0 G90 Z2.0

G91 G28 Z0

G103 ( Activate  Look Ahead )

M30

On the p9820 line I'm not sure what my Z should be.....the Z.25 will locate the probe .25 above the previous  Z0

Am I in the ball park with this.

Just so we are on the same page. After probing the 4 locations in Z, I want the biggest Z # to become my G54 Z work offset #.

Thanks for any input

Mike

So when i ran the code i ended up getting a 1092 open probe alarm as soon as it reads G65 P9820 line

I tried to upload a pic but it errors out

File is small enough

I can email the pics if anyone has time to look

Thanks Mike

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • 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.

Follow us