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:

In-process inspection and probing in Mastercam


Recommended Posts

We are running FactoryWiz on our machines to collect run data.

Part of this is taking in-process probing data and outputting/formatting to an IPI (In-process Inspection) report.

We have multiple machines with Renishaw probes (Haas, Brother, Makino, and Grob)

Trying to decide which way to go for programming the probes,,, We have the Productivity+ add-on in Mastercam but have not implemented it yet.

My concern is it writes ALL the macros into every program you post, this makes for huge files that seem unnecessary.

I have seen other software out there: Camaix Probe Manager, Cimco Probing, and there are probably others.

Looking for some feedback on what everybody runs and how they program probes in Mastercam (I need verification/simulation also)

Link to comment
Share on other sites

Hi Kevin,

Outputting the actual Subroutines for the Probe Calls, is only the default. You can easily turn off that output, and only output the Macro calls themselves.

Talk with your Reseller, and get a copy of the Renishaw Productivity Plus Configuration Tool, which is used to configure the RenMF file for proper output.

Are you only Inspecting and Outputting the data, or are you measuring/recutting as well?

The reason I ask is that Productivity  Plus can also be configured to output sequence blocks (start/end markers) in the Program. You can cut a feature, output a measuring macro call, with feature tolerance zones, and if the feature is still "stock on", the logic can output a G10 Wear Offset update, then jump (GOTO) back to the restart block, and re-cut the feature, then re-inspect, and throw the standard errors if the feature is not within tolerance.

Are you interested in bringing in someone to help with implementing Prod+ in your shop?

  • Like 2
Link to comment
Share on other sites

Outputting just the macro call is the way to roll.

A "gotcha" you need to keep an eye out for when you have multiple machines is that many machine builders are using their own version of renishaws inspection plus macros, with the same macro number, but they work "basically the same", which translates to sometimes they don't work worth xxxx. Also some controls can't deal with equations that have two sets of negative values.

It is critical that all your machines are running genuine Renishaw inspection plus macros, and that you have tested that  tool wear compensation values get applied in the correct direction on each machine.

 

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
3 hours ago, Sticky said:

It is critical that all your machines are running genuine Renishaw inspection plus macros, and that you have tested that  tool wear compensation values get applied in the correct direction on each machine.

Very well said!

To be able to get to this point though > someone has to take the time to verify 'which Macros' are running on each machine, and do the work to make sure all macros are functionally the same.

Based on when the macros were written (or modified) by Renishaw, there can be several differences:

  • In general, the "basic measuring functionality" will all be the same. Some users never get beyond this level of implementation, and that is OK, if it works for them. The "newer" versions of the Renishaw Macros, will include dozens of "internal macro calls", which end up "preparing the variables, so that the Macro runs correctly". An example of this would be > at the start of a Circle Measuring Call (G65 P9814), contained within the 9814 Subroutine itself, will be a "Probe On" Macro Call, as the first "jump" encountered. (There may be preparatory G-codes or M-codes present, but this will generally be the first, or at least a very early, Subroutine Jump.) In that Probe On Macro Subroutine Program, there will be other Subroutine Jumps, which are used in the modern versions of the Inspection Plus Macros, to do things like "load the Calibration Variables", so that all the variables are set, before the actual Circle Measuring takes place.
  • So, if you are just looking for "measuring something", or "setting a Work Offset", then you can usually get away with having slightly different Subroutines on the machine, provided that you only pass certain Parameters to the Macro itself. An example of this, again, can be made with the Circle Measuring Macro. If all you want to do is set a Work Offset, then you only need to provide certain Parameters to the Macro, and it does what you what it to do. But, you give up the ability to know with confidence that you can also use the more advanced features like 'Custom Probe Over-Travel Distance', 'Feature Tolerance', 'True Position Tolerance Zone', or 'Update Tool Offset'. These options are invoked by using "optional parameters" on the Macro Call Line, but you must ensure your Macros are actually setup to use all of these optional parameter values.
  • Look at the difference between these two Macro Call Lines:
  1. G65 P9814 D50.005 Z100. E0.005 F0.8 H0.2 M.2 Q10. R10. S1. T20. U.5 V.5 W2.
  2. G65 P9814 D50.005 Z100. S1.
  • Line 1 contains all of the 'optional input parameter values'. This Macro is setup to Probe an External Boss, with both a Feature Tolerance and a True Position Tolerance. By passing these additional Parameter Values, the '9814' Macro will use different 'conditional jumps' within the macro body, to execute additional Subroutines > as a result of passing these additional Parameters.
  • Line 2 contains the two required or obligatory Macro Parameters: 'D' and 'Z'. You are only required to pass these two Parameters to allow the cycle to execute. (Fun fact: the subroutine will throw an alarm if any of the 'required' parameters were missing when you called the Subroutine.) It also contains a third parameter: 'S'. The "S1." tells the Macro to update the Work Offset XY Location, of the G54 Work Offset. It does this automatically, after it finishes measuring the Bore. Wait > how did I know this Macro Call, would measure an internal feature, when the first example line measured an "external boss"?  The answer is that every Macro has a default behavior when certain Parameters are omitted. This will be explained in the Renishaw PDF Files, that are specific to the particular Probing Package that you either purchased, or that came installed with the machine.
Link to comment
Share on other sites

Is this where the RenMF would control each machine type ?

Our Brothers have Renishaw probes but there are differences in the macros from the Haas machines (which are all the same)

The Makino cell will be a different animal. We will tackle this one after the verticals are dialed in.

Our new Grob has a Siemens control and I have not had a chance to look at the probing yet. (still setting the machine up)

Link to comment
Share on other sites
4 hours ago, kccadcam said:

Is this where the RenMF would control each machine type ?

Our Brothers have Renishaw probes but there are differences in the macros from the Haas machines (which are all the same)

The Makino cell will be a different animal. We will tackle this one after the verticals are dialed in.

Our new Grob has a Siemens control and I have not had a chance to look at the probing yet. (still setting the machine up)

Yes, certainly a unique RenMF file for each Machine/Control type, and a unique RenMF file for any machine that doesn't work like the others.

Also, it's possible to have several RenMF Files for a single machine, each with a different configuration. 

Link to comment
Share on other sites
  • 2 weeks later...

Hello,

I started reading this post and I am finding it very interresting.

If I understand correctly, you can output production plus macros to the Nc program by configuring the RenMF file.  Is this correct?

Does it work with the productivity+ module?

 

I am very interrested to see what can be done.  My boss wants this so badly.

 

Regards,

 

Martin

 

 

Link to comment
Share on other sites
On ‎4‎/‎10‎/‎2019 at 6:17 PM, Colin Gilchrist said:

Hi Kevin,

Outputting the actual Subroutines for the Probe Calls, is only the default. You can easily turn off that output, and only output the Macro calls themselves.

Talk with your Reseller, and get a copy of the Renishaw Productivity Plus Configuration Tool, which is used to configure the RenMF file for proper output.

Are you only Inspecting and Outputting the data, or are you measuring/recutting as well?

The reason I ask is that Productivity  Plus can also be configured to output sequence blocks (start/end markers) in the Program. You can cut a feature, output a measuring macro call, with feature tolerance zones, and if the feature is still "stock on", the logic can output a G10 Wear Offset update, then jump (GOTO) back to the restart block, and re-cut the feature, then re-inspect, and throw the standard errors if the feature is not within tolerance.

Are you interested in bringing in someone to help with implementing Prod+ in your shop?

Colin - you seem to have a lot of knowledge on the subject of in-process on the machine inspection probing using mastercam. This is something our shop does using PC-DMIS currently and I am trying to get the probing programming of the CNC machines moved into the programming dept. instead of being done by the quality dept. I am interested in training and configuration of the software to get this done.

What do you offer as far as training and configuration?

Thank you,

Tim

 

Link to comment
Share on other sites
5 hours ago, MetalSlinger5 said:

Colin - you seem to have a lot of knowledge on the subject of in-process on the machine inspection probing using mastercam. This is something our shop does using PC-DMIS currently and I am trying to get the probing programming of the CNC machines moved into the programming dept. instead of being done by the quality dept. I am interested in training and configuration of the software to get this done.

What do you offer as far as training and configuration?

Thank you,

Tim

 

 

Hi Tim,

I can offer as much, or as little training as needed, depending on the particular needs of your business.

I have been doing quite a bit of Productivity Plus Implementation lately, which really involves a couple different steps:

Implementation

Implementing Productivity Plus in any shop involves a couple different tasks:

  1. Modifying the Mastercam Post Processors (depending on their original "vintage" or build date), to be "configured for Prod+ Support". There is a PDF Document, contained in the Mastercam Post Processor Documentation, that walks you through the process of making these modifications. For me, this is roughly 10-30 minutes of work, per Post Processor, to make the necessary changes to support Probing. But that is only the very 1st step. It also highly depends on if you: 1.) Just want me to do the work for you, or 2.) want me to teach you how to make these modifications in the Post(s), so that you can do the same work for new machines in the future...
  2. Once the Mastercam Posts are configured, we then tackle Configuration of the Renishaw Machine File (.RenMF). It takes (me) about 2-3 hours to configure a Renishaw Machine File, with teams that are already familiar with the Probing Process, the on-machine Macros being used, and Probing in General. I have also taken an entire day to focus on the 1st machine being configured, because the users had never done Probing before, and we had to figure out "what macros, variables, and processes were already in-use".
  3. Once the 1st RenMF file has been configured, it is typically a 2-3 hour process, per Control Type, to do the rest of the RenMF Files. However, I have had shops where we ended up having to create a unique RenMF File, for each specific machine, since there were differences between how each machine had originally been setup.
  4. Once the Mastercam Posts, and Renishaw Machine Files have all been configured, I then generally do training on the Renishaw Prod+ "Toolpath Interface" in Mastercam. This typically takes a half-day (on the low-end), to two full days (on the high-end), to get everyone comfortable with the "Mastercam side of the Process".
  5. Then, we typically do some "on-machine" training, running through Probe Calibration, Setting Work Offsets, and executing Measuring Cycles with the Probe.
  6. Finally, we will do some investigation into "what kind of output options are available on the machine", and finish with configuring the "Probe Measuring Results, formatted in some kind of Inspection Report Format". Typically, we involve the Machine Tool Builder for this part of the implementation, since each machine (and shop) has unique requirements.

Training

This can be for several "Programmers", and usually involves showing them the Mastercam Process for creating the Probing Cycles. I will usually also cover some things like Boolean Logic (Fanuc Style), and Conditional Branching.

The Prod+ interface gives us the ability to create "custom Sequence Blocks", with "GOTO" statements to control Program Flow. Much of the "Training" will also depend on what gets covered "during implementation".

I have done Training/Implementation together, when the shop is small, with only 1-2 users and/or machines. However, the training and implementation needs grow exponentially, as the number of machines and programmers grows.

 

It sounds like you've already got quite a step up, since your Inspection Department is already executing (poorly) the inspection processes with PC-DMIS, which will make the transition to Prod+ actually fairly straightforward.

Please send me an email, so we can discuss your needs, and I can put together a custom quote for your shop.

[email protected] or [email protected]

Thanks and best regards,

Colin Gilchrist

 

  • Like 3
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

  • 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

×
×
  • Create New...