RENISHAW PRODUCTIVITY+ ISSUES

[Stockyrock]

Hi everyone,

We just bought Renishaw Productivity Plus for Mastercam X7. I am trying to make it works on our new machine :

machine: AWEA 3016

controller: FANUC 31i

 

The dealer modified our post .pst to make it communicate with the Renishaw post ,renmf for FANUC 31i controller. On MasterCam, I am able to post the program. However, when I am trying to run it on the machine, the program tries to open subprogram that doesn't exist on the machine (see the attached file to see all the program that the program is trying to open.

 

Here's the beginning of the program until the error pop on the screen:

 

O0000 (PIECE TEST-6)

(AWEA SP3016)

(MACHINE GROUP-1)

(MCX FILE - G:\RENISHAW PROBING\PIECE TEST.MCX-7)

(PROGRAM - PIECE TEST-6.NC)

(DATE - DEC-18-2013)

(TIME - 11:16 AM)

(T60 - RENISHAW OMP60 - H60 - D60 - D0.2362" - R0.1181")

(T4 - SLOTTER 1.00 COURT R1/16 PASSE .125 - H4 - D4 - D1.0000" - R0.0620")

(T48 - END MILL 3/8 .375 CARB. FINISH - H48 - D48 - D0.3750")

#149=0 (RENPROGSTART)

#148=0 (RENPROGSTARTEND)

(_RENGCODE_START0001)

 

 

 

N100 G00 G17 G20 G40 G49 G80 G90

(_RENGCODE_END)

 

 

 

(PRODPLUS_BEGIN)

POPEN

DPRNT[]

DPRNT[PROGRAM*START*PGS]

DPRNT[**REPORT*VERSION*1F]

DPRNT[**PROGRAM*NAME**O]

#1=FIX[#3011/10000]

#2=#3011-[#1*10000]

#3=FIX[#2/100]

#4=#2-[#3*100]

DPRNT[**DATE*#4[20]**#3[20]*#1[40]]

#1=FIX[#3012/10000]

#2=#3012-[#1*10000]

#3=FIX[#2/100]

#4=#2-[#3*100]

DPRNT[**TIME*#1[20]**#3[20]**#4[20]]

PCLOS

M5

G54

G90 at this line FILE NOT FOUND POP

G65 P2109 A1. C1. I0. 1181 D2. E2. H60. M0. Q0. R0.T-999U60.V1.W0.91Z1.

 

Right now I called the dealer where we bought the machine, they said that all the program are in the machine... I called the dealer who sold us Productivity plus and they don't know why it doesn't work... I also wrote to Renishaw and I am waiting for a response. I also check every single program in the machine..

 

Can anyone help me ?

Thanks a lot

Cedrick Baker

Missing Sub Programs AWEA 3016.txt

[Colin Gilchrist]

In the RenMF file you can set the value for each Subprogram that gets called. Can you find out from your Machine Dealer what those macro numbers are? Once you know what the numbers are you can set them in the RenMF file to use those macro numbers.

 

We made some changes recently to let a user call an existing Macro on the machine's control. The "normal" output we create for Prod+ will post out each macro as a sub program, and the sub will be listed after your main program. This is to prevent errors where the Macro on the machine is out of sync with the Macro output from Prod+.

 

You'll need to work with your Reseller on these issues, and may need to upgrade to X7 MU1, to get the fix for outputting macros separate from the main program...

[Chris Bloedorn]

You should be able to get your Renishaw contact to give you a copy of all the Macro's to load on your machine. With each new version of P+ you will likely need to do this to make sure nothing has changed....

[Guest]

P2109 is NOT a Renishaw MACRO.

 

What are you maesuring?

[YoDoug®]

P2109 is NOT a Renishaw MACRO.

 

What are you maesuring?

 

Renishaw defaults the inspection plus macros to 2*** in their productivity+ posts. Open the Prod+ post and there is a section where it sets the macro numbers or change the name of the 9*** macros in the machine control to match. They should all be just the first digit to change, IE, 2109 to 9109

[Stockyrock]

I called our Dealer and they provide me a working .RENMF. So now I post also all the macro needed for the program (about fifteen). However, It seems that the controller cannot read a subprogram...

I tried to make a file for each macros, put it in the CNC MEMORY and the controller still don't find the macros...

 

For a Fanuc 31i Controller, is it the right way to call a subprogram : G65 P2109 A1. C1. I0. 1181 D2. E2. H60. M0. Q0. R0.T-999U60.V1.W0.91Z1 ?

[RayD]

Have you run the Configuration from P+? It uses different Macros and variables than the supplied macros that come on the machine.

[Masterminder408]

Renishaw defaults the inspection plus macros to 2*** in their productivity+ posts. Open the Prod+ post and there is a section where it sets the macro numbers or change the name of the 9*** macros in the machine control to match. They should all be just the first digit to change, IE, 2109 to 9109

 

You can request "Productivity plus post configuration" from your reseller, that will enable you to change all the sub program 's number, I changed all mine to start at #8000 only to avoid confliction with others, same as all variable values. There is a configuration inside "Renishaw pst config" that will enable you to out put all sub with main program.. you must have that turn off...

 

ohh one more thing, after changes made, make sure that you run the "Proble Calibration" using all new sub and variables value.. it will store the differential error of probe needle...

[Stockyrock]

Thanks for the help! I solved THIS problem (So this mean that there is another problem...).

 

First of all, if you got the same problem with a similar controller here's how I add MACROS to the CNC MEMORY:

1-Post your program

2-Separate each MACROS in the main program

3- Name the files OXXXX.NC (where X's are numbers)

4- Transfer all the MACROS in a USB key (this is the only way that works for me, I cannot do it using our SERVER)

5-Connect the USB to the Controller

6- EDIT MODE

7- OLIST> IN/OUT

8- Now you are supposed to be in the USB KEY

9- Find the first MACRO you want to input in the CNC MEMORY

10- IN/O

11- They will ask you to change the name, name it OXXXX (MACROS don't have .NC)

 

Voila!

 

 

Here's my new problem:

When I start the program, I got the following error: 3100 REN11.PROBE*SWITCH*ON*ERROR

 

BEFORE the error, the machine change his tool for the probe, goes near MACHINE ORIGIN, and it seems to try to teach a zero there... and the probe is supposed to go over the piece and teach the Z0. I don't really understand because I already teach approximate zero to tell the machine where the piece is, so it should go at this position.

 

Anyone has an idea of the problem is going on ?

[Masterminder408]

How was your probe setup ?you have to calibrate your probe with Productivity plus calibration cycle first before you do anything

[Stockyrock]

What do you mean ? my probe is already calibrate (using EASYSET from Renishaw). Do you mean that I have to do it each time I want to use productivity plus ?

[crazy^millman]

He is asking did you follow his instructions on the process. Think of this as a new start and the probe is brand new never cal raised now.so everything needs to be taught again. Right now you are using all brand new variables and macro routines and everything needed to make those runs needs to be taught to the machine again. Yes I understand you think no, but unless you copied every value piece by piece from the old places to the new places then yes you need to rerun the calibration routines with all the new settings and you should be good to go. Welcome to the wonderful world of using a probe on a machine tool.

 

HTH

[Stockyrock]

I just found that the 3100 REN11.PROBE*SWITCH*ON*ERROR appeared simply because in the MACROS there was no M-Code to turn on the Probe RECEIVER. So I simply add it using the Post Process. Conf.

 

When I restart the program, another error shows up : 3106 REN17.STYLUS*OFFSET*POSITION*ERR. Now it really looks like the probe needs to be calibrate using PRODUCTIVITY+ macros.

 

Thanks Masterminder408 for the tips and Crazy^Millman for the tip's explanation

[Stockyrock]

I have done the probe configuration : ring gauge and reference surface. 3106 REN17.STYLUS*OFFSET*POSITION*ERR don't show up.

 

However, I go further in the program and 3100 REN11.PROBE*SWITCH*ON*ERROR has reappeared... I don't understand why.

[Masterminder408]

Check this out,

 

" Be very careful"

 

This is for a Haas 's Probe, so your machine could have different code...

 

This is an example ONLY...

[Colin Gilchrist]

Mastermind is correct Stocky. You will most likely need to add the "probe on" codes to your RenMF file. The easiest way to do that is by using the configuration utility from Renishaw (available from your Reseller). If you aren't sure what that code should be, please contact your local Renishaw AE, and they will be able to get you sorted out.

 

Hope that helps,

 

Colin

[Kenny Machado]

Hello everyone,

I have tried to post a Renishaw routine and my Mastercam simply crashes.

 

Well, my mastercam .PST is already enabled to accept Renishaw post-processing routines.

I can start any application into Productivity+ and ask to create the G-Code. After that mastercam will process its information and Renishaw post options box opens up. 

I select my .RenMF and click in "Process", at this point my Mastercam closes automatically.

I have tried several times, changing part of the process, using all the strategies available in my P+ but the results were the same.

 

I verified then that a LOG ERROR appeared to me, into PROBEDATA folder (C:Users/Public/PublicDocuments/SharedMcam/Commom). Which is bringing the information that several macros in P+ are designed for CNC Plug-in use only. And that the current set up is Macro-Mode.

When I asked a Renishaw salesperson I was said that is EXACTLY THE OPPOSITE, all custom macros are designed to be used with Macro-Mode, not Plug-in.

So, I continue without being able to use P+ functionalities.

 

Attached below is the LOG ERROR I found in PROBEDATA folder.

If someone has already experienced this and knows how to solve it, please, will help me a lot!

ProductSupportErrorLog.txt

[Colin Gilchrist]

On 9/28/2018 at 1:24 PM, Kenny Machado said:

Hello everyone,

I have tried to post a Renishaw routine and my Mastercam simply crashes.

 

Well, my mastercam .PST is already enabled to accept Renishaw post-processing routines.

I can start any application into Productivity+ and ask to create the G-Code. After that mastercam will process its information and Renishaw post options box opens up. 

I select my .RenMF and click in "Process", at this point my Mastercam closes automatically.

I have tried several times, changing part of the process, using all the strategies available in my P+ but the results were the same.

 

I verified then that a LOG ERROR appeared to me, into PROBEDATA folder (C:Users/Public/PublicDocuments/SharedMcam/Commom). Which is bringing the information that several macros in P+ are designed for CNC Plug-in use only. And that the current set up is Macro-Mode.

When I asked a Renishaw salesperson I was said that is EXACTLY THE OPPOSITE, all custom macros are designed to be used with Macro-Mode, not Plug-in.

So, I continue without being able to use P+ functionalities.

 

Attached below is the LOG ERROR I found in PROBEDATA folder.

If someone has already experienced this and knows how to solve it, please, will help me a lot!

ProductSupportErrorLog.txt

Contact your Reseller for support. Are you running a standalone Hasp or a NetHasp? It looks like a licensing issue...

[Ewood42]

Trying to set up Productivity+ here at my new job. Hitting a pretty big snag. The sub (originally labeled 2109) turns on the probe, but does not seem to confirm the probe is on. Keeps trying to make a G31 move looking for a skip signal, doesn't get it because it's still up just below machine zero, then repeats the power on code. Any thoughts? The install was halfway done when I picked it up so I'm guessing I may need to go back and change some settings that were made before I picked it up, but not sure where to start. Any ideas? Just trying to run the calibration cycles, but 9109(2109) is the first thing it calls.

I did take the time to match up all the probe calibration values from the existing probing cycles, but it won't even verify the probe is on at this point.

[Chally72]

Hey Ewood,

I'm the one working with your reseller on this. I sent some initial questions along this morning that you should see soon, if you haven't already.

To clarify here- Productivity+ does NOT use the same variable sets as Inspection+, nor does it use the same macros that you see at a controller level on a machine that has Inspection+ installed. Productivity+ has its own separate calibration cycle that must be posted from Mastercam that uses a separate set of variable blocks to store info. In short, with what you've mentioned with an old half-done install, we'll probably slowly back away and come back at this like a fresh install. 

[Ewood42]

2 hours ago, Chally72 said:

Hey Ewood,

I'm the one working with your reseller on this. I sent some initial questions along this morning that you should see soon, if you haven't already.

To clarify here- Productivity+ does NOT use the same variable sets as Inspection+, nor does it use the same macros that you see at a controller level on a machine that has Inspection+ installed. Productivity+ has its own separate calibration cycle that must be posted from Mastercam that uses a separate set of variable blocks to store info. In short, with what you've mentioned with an old half-done install, we'll probably slowly back away and come back at this like a fresh install. 

Oh, I see. I wonder if that was my problem. I tried to set up the .renmf file to point to the same calibration data being used by inspection. One of my co-workers said they thought that's how it had been set up in another shop they worked at - so I assumed I could at least get the two sets of software to share that data.

 

So I need to find a set of variables not being used by inspection plus or any other functions to use for the prouctivity+ calibration data?

Also, should I be using the inspection plus power on code in my .renmf file (p9832), or the M59/M69 Pxxxx codes being used by inspection+?

[Chally72]

Hey Eli, 

I sent another round of instructions to your reseller, but to answer some of these here for anyone else looking:

-Yes, we will be using #656-675 by default as calibration variables for Productivity+ to keep this separate from the Inspection+ calibration variables. The Productivity+ calibration is different/more extensive than for Inspection+, and they must be treated separately if both sets of macros are to work properly and accurately. It looks like that RENMF was an older file and also heavily edited, so I sent along a default one for 2020, and we'll start from there to try and reduce the number of setup issues we're running into here. G65 P9832/P9833 are default switch on/off. 

 

[Ewood42]

Thank you! That was the nudge I needed in the right direction. It worked on the VF5SS, just took a bit to figure out the MCAM side of it. Got it set up and working first try on one of our older haas machines.

How difficult is it getting the multi-axis functionality working?

[Chally72]

Oops, almost missed this! As you've kind of seen, this could be very quick or it could be an extended amount of time standing next to the controller working things out. It's a short section of the RENMF to turn things on and set it up. I'd definitely work with your reseller- we have programming examples they can share that will give you a good feel for the Mastercam end of things.

[Colin Gilchrist]