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:

Tool break test


johnr4mbo
 Share

Recommended Posts

Yeah that's what I was thinking too. Wasn't sure where to add it in inside Mastercam. Might need to check your Renishaw program numbers for Haas but manually add in manually until your post is updated. I stole this from another forum but it should be something similar:

"At the end of the tool cycle enter:

G91 G28 Z0;
G90 G49;
G65 P9853 B1. T#3026 H.02;
M1;

H being your tolerance on the length. #3026 is the variable for what tool is currently in the spindle. You can substitute it with the numeric value if you wish."

It might not be 9853. I'd look through your cycles. There's a couple different ones too and I believe P9853 feeds down to the probe. There might be one that rapids to like .25 above it. 

Link to comment
Share on other sites
1 hour ago, Matthew Hajicek™ - Conventus said:

I had Postability add a Misc Real for tool breakage detection.  Zero is off, any other value is the tolerance for the break check.

I'm planning on having my re seller add this to my post. How did you end up handling on center detection vs diameters greater than .375?

Link to comment
Share on other sites
Just now, Tinger said:

I'm planning on having my re seller add this to my post. How did you end up handling on center detection vs diameters greater than .375?

I don't, I just use it for on center detection.  It's mostly for drills, so I don't jam another tool in after a broken drill, and occasionally for endmills.  I would have to hand edit for a shell mill.

Link to comment
Share on other sites
43 minutes ago, Tinger said:

I'm planning on having my re seller add this to my post. How did you end up handling on center detection vs diameters greater than .375?

Read up in your Renishaw Manual on the "input variables" available to the Probe Cycle. 

Most of the Probe Cycles have 'optional parameters', which cause the Probe Cycle to behave differently, depending on the actual parameters that get passed with the Probe Macro Call.

Typically, there would be a "diameter" value that would get passed on the G65 line, which would allow the Program to offset the tool by the tool's radius, so that the teeth of the cutter contact the Probe Tip.

The Renishaw manuals are all organized in the same way. At the beginning of the Manual, there will be a section that describes in detail, all of the "Optional Inputs" to the cycles. There will also be a "Variable Output" section, which lists the #100-#149 "output" values, from each Probe Cycle. (outputs also vary, depending on the specific inputs to the macro program being called.)

In general, it is simple for the Post Developer to just output either the Tool Diameter or Tool Radius, as a Parameter that is output on the G65 Macro Call line. The actual Measuring Macro developed by Renishaw should take care of the rest on its own.

  • Like 1
Link to comment
Share on other sites
8 hours ago, johnr4mbo said:

Hi,

 

How do i break test a tool for length with Mastercam?

 

Thanks in Advance,

Rick

Do you have this product here: https://www.mastercam.com/solutions/productivity/, Mastercams productivity+ software? That's the easy way to do it in my opinion, its done in just a few clicks to apply Tool Breakage detection through Mastercams productivity+probing toolpaths. 

Edit: if you do have productivity+ let me know what machine your doign it on and i can put together a short video showing how to use Mcam Prod+ to do tool breakage detection.

 

Link to comment
Share on other sites
3 hours ago, Colin Gilchrist said:

Read up in your Renishaw Manual on the "input variables" available to the Probe Cycle. 

Most of the Probe Cycles have 'optional parameters', which cause the Probe Cycle to behave differently, depending on the actual parameters that get passed with the Probe Macro Call.

Typically, there would be a "diameter" value that would get passed on the G65 line, which would allow the Program to offset the tool by the tool's radius, so that the teeth of the cutter contact the Probe Tip.

The Renishaw manuals are all organized in the same way. At the beginning of the Manual, there will be a section that describes in detail, all of the "Optional Inputs" to the cycles. There will also be a "Variable Output" section, which lists the #100-#149 "output" values, from each Probe Cycle. (outputs also vary, depending on the specific inputs to the macro program being called.)

In general, it is simple for the Post Developer to just output either the Tool Diameter or Tool Radius, as a Parameter that is output on the G65 Macro Call line. The actual Measuring Macro developed by Renishaw should take care of the rest on its own.

To check a diameter larger than .375 , all I have to do is add a D .XXX value to my M165 line. (Doosan custom renishaw maco insetad of G65). I was just wondering how you would implement that on the misc variables page. Maybe add the dia to the corresponding real input? Say misc integer 0= no breakage cycle, 1= breakage cycle. Then in the reals numbers you could add the diameter; 0= on center then any other value would output as the D.XXX?

Link to comment
Share on other sites

Check out these Smart phone apps for Probing, i have them on my Android phone and they are pretty cool and might be useful to you, i am not sure if its on the Apple app store has them or not but these are free and fore sure in the Android app store. GoProbe gives you some probing cycles, i dont see a tool break cycle in there but there is some other cycles for some standard controls.

  • GoProbe
  • Trigger Logic
Link to comment
Share on other sites

there should be a way to pull the tool diameter from one of the master can parameters. But I have no idea how to do it.

 

I was able to do it through camplete using miscellaneous integer one for drill two for Endmill.  Then the miscellaneous real next to it is used for tool break tolerance. And the format macro for the endmill inserts the value for the camplete cutting tool diameter parameter 

  • Like 1
Link to comment
Share on other sites
1 hour ago, Leon82 said:

there should be a way to pull the tool diameter from one of the master can parameters. But I have no idea how to do it.

 

I was able to do it through camplete using miscellaneous integer one for drill two for Endmill.  Then the miscellaneous real next to it is used for tool break tolerance. And the format macro for the endmill inserts the value for the camplete cutting tool diameter parameter 

tldia$ works in MP-based Post Processors for Mastercam.

tcr$ gives the Corner Radius

  • Thanks 1
Link to comment
Share on other sites
  • 5 months later...

Just found this topic through a search.

We have been using Productivity+ for maybe five years or so.  Early on I tried to use the Tool Break Detection feature in Prod+ but never got it to work.  I'm using it on a Haas VM2.  Last week I watched a webinar on Prod+ and saw some new info on using the Tool Breakage Detection feature, so I tried it again with what I learned from the webinar.  Still didn't work.  I contacted my reseller and explained the situation.  Sent him a Zip2Go and my RenMF file.  He worked on it a bit but could not get it to work.  He forwarded it to CNC Software.  They came back with a couple of suggestions but it still didn't work.  It went a couple of days and my reseller told me CNC Software was still working on it.

I am able to post code and run the program on my machine.  I did a test where I did a simple contour then measured the tool.  It ran the contour, then moved over the probe pad, came down and hit the probe pad, and then gave the alarm "Probe Open".

NO JOKE - as I was typing this my reseller e-mailed me again asking if I was able to run other Prod+ toolpaths on my machine or was the Tool Breakage Detection was the only one I have tried.  Told him I've been using it for years, but never got the Tool Breakage Detection to work.  I guess CNC Software really is still working on it.

  From my Reseller:   Are you able to post other Productivity + toolpaths that run on your machine is this the only one that you have tried? 
  Thank you,
  XXXXX XXXXXXX
 Applications Expert

Does anyone here have a suggestion of something I can try?  I see JoshC above may have some ideas.

Link to comment
Share on other sites

Hey LA CAMmer,

I'm the one that your reseller has been emailing- I got involved last Friday after CNC Tech Support forwarded it to me and we've been going back and forth. I just sent some additional requests to him, but if you can provide me the NC file that you're actually running at the machine, that would be very helpful- it's the one thing I'm missing. (Just a note- he's been on top of it- if anything, I've been the delay in response times since Friday)

-Have you reloaded the macros onto the control since you've updated to 2019? Renishaw switched from v2.1 to v2.9 macros and 2019 is when the switch was made for Mastercam Posting.

-Additionally, the vanilla release of Mastercam 2019 contained an error with the installed location of probing files, and thus it would default to older Renishaw v2.1 files instead of v2.9, and this causes many issues, but more importantly, you may never see it if you're running only features that didn't change between v2.1 and v2.9. There’s a KB article here on how to fix this, and it’s important to follow it, because if you don't want to do the manual steps noted, doing a patch update instead of a complete uninstall and fresh reinstall with a full update EXE will not solve this issue on its own:  https://kb.mastercam.com/KnowledgebaseArticle50610.aspx?Keywords=productivity

 

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

Is there a chance the eye is obstructed?

Good point that I forgot about, Leon82. In our shop, the tool probe in the VF2 stopped working after a certain time of day every day- the sun was whiting out the sensor.

Similarly, the lighting in the new UMC-750's is great, but if angled perfectly (or incorrectly) in a shiny new machine, it'll white the sensor out when the spindle head comes down.

Since this gentleman's probe works file for setting tool lengths, this is probably not it, but it's good feedback for people having problems.

  • Like 1
Link to comment
Share on other sites
29 minutes ago, Chally72 said:

Good point that I forgot about, Leon82. In our shop, the tool probe in the VF2 stopped working after a certain time of day every day- the sun was whiting out the sensor.

Similarly, the lighting in the new UMC-750's is great, but if angled perfectly (or incorrectly) in a shiny new machine, it'll white the sensor out when the spindle head comes down.

Since this gentleman's probe works file for setting tool lengths, this is probably not it, but it's good feedback for people having problems.

Same think with us, the raptor base plus dove tail and workpiece added up to erratic open alarms.  

We twisted the housing on the ots. There are about 7 holes to pick from and index it

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...