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:

Program numbers for Renishaw probing macro software


Recommended Posts

Hello eM,

We have a lot of used machinery with different probes and receivers - and different technicians.

Among the Fanuc controllers, there appears to be a lot of macros that do identical things, such as three-point-bore routines, but have different program numbers. All of them are in the 9000 range though.

Thus far none of them are documented, so we are not sure if they were custom written, or from a Renishaw package such as 'Inspection Plus'.

Is there a standard numbering system that Renishaw uses for its macro programs?

Haven't found anything in their documentation, and they are obviously gone for the holiday weekend.

Sorry in advance if anything was overlooked.

Thank you

Link to comment
Share on other sites

The probes and receivers came with the machines when they were bought from various auctions, and did not come with any hard copies of Renishaw's documentation. When I said documentation I was actually referring to Renishaw's website. Next week we will contact both Renishaw and our technicians, but in the meantime the hope was to gather any bits and pieces of information from the user communities.

Do you happen to know which Renishaw software package you are using? Are you referring to Renishaw's website or to hard copies of the documentation? Any feedback would help.

Thanks

Link to comment
Share on other sites
22 minutes ago, Leon82 said:

They are usually 9510 or 9810 and go up from there I think

So for example if a simple Z touch-off routine is program 9555, can that same program number/routine be found in all of Renishaw's machine tool probing packages, or are the program numbers only relevant to the specific package that you buy from them?

Link to comment
Share on other sites

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

These are probably the most "standard" numbers in use for the Renishaw Probe Cycles. I say that based on the sheer number of Haas machines that have been sold with a Renishaw Probe over the years. This package uses O9810 for protected moves, O9811 for single surface probing, O9812 for web/pocket, and O9814 for Bore/Boss.

Keep in mind that the Probe cycles themselves can be re-numbered, for all sorts of reasons. The fact that you've bought some of these machines at auctions, means that you'll need to review what Macro Programs are currently installed on each one.

That Renishaw manual from 2008 has all the information needed to get a good understanding of the Probe cycles and Parameters (arguements) which can be passed on the Macro call line. Remember to always include a Decimal Point (.) After each argument/parameter.

  • Thanks 1
Link to comment
Share on other sites

Here's the Renishaw InspectionPlus manual. I believe it's the most current. If it's not, there's only subtle differences.

PQI usually uses O95nn to avoid conflictswith Machine Tool Builder MACROs. Most Renishaw installations however stay true to what's in the Renishaw manual (O98nn) 

#135 - #149 Variables never change AFAIK.

https://www.dropbox.com/s/tlv3673fvuxssvf/H-5755-8600-03-A - InspectionPlus Manual.pdf?dl=0 

 

  • Thanks 1
  • Like 2
Link to comment
Share on other sites

I would be leery of the odd macros in your control. I for one have taken Renishaw macros and modified them to do one specific task on a specific part and saved it as a different program number. Renishaw does have specific program numbers across a wide range of machine tools. I would start with the Renishaw manual, keep those programs and discard the rest and start from scratch. You have no idea how the odd macros were modified and in some cases you would not like the result.

 

Paul

  • Thanks 1
Link to comment
Share on other sites
On 12/1/2020 at 11:04 AM, PAnderson said:

I would be leery of the odd macros in your control. I for one have taken Renishaw macros and modified them to do one specific task on a specific part and saved it as a different program number.

Thanks - yes it appears that is precisely what happened. There seems to be a mixture of modified programs and standard ones. It appears that the best option is to start over by installing the latest version of Inspection Plus, but it's still not entirely clear which of these macros the machine relies on. Once we sort it out we should be able to start from scratch.

Link to comment
Share on other sites

Looking through the Inspection Plus Manual, it appears that the probe calibration process is a 3 part procedure: 1) stylus offset (XY), 2) stylus radius, and 3) probe length (Z). Looks like each step uses the same macro program 9801. Are these steps usually done as three separate calls, even though they use the same program number? Obviously calibrating Z would require a repositioning move.

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...