So not a Guru

Odd threadmill action in 2018

Recommended Posts

This might just be how it works, but I seem to remember doing this in earlier versions differently.

I have a threadmill with 1/8" of flute lenght and 7/8" of extended reach, and I'm threading .40" of depth.

The path is broken into 3 separate vertical sections, instead of screwing all the way from bottom to top. Am I missing something in my settings?

I've attached a pic showing what I'm getting on the left. Ignore the paths to the right, they're made by the full length threadmill that hasn't gotten to our facility yet:rant:1459951730_THREADMILLISSUE.thumb.PNG.c4f6d8134abb275941cd08ebc1964712.PNG

 

Share this post


Link to post
Share on other sites

Tell it the tool has one tooth in the operation and it will machine from bottom to top.

Share this post


Link to post
Share on other sites
13 minutes ago, 5th Axis CGI said:

Tell it the tool has one tooth in the operation and it will machine from bottom to top.

Thanks Ron, I knew I made it work correctly before. I've slept at least twice since then, so my oldtimers wipes that memory away. 🤪

Share this post


Link to post
Share on other sites

I don't remember what but I have two R-#s on threadmill in 2018.  One was the displayed toolpath is incorrect but posted correctly.  That may be what you're seeing there as it is similar to what I recall.  The other was on migrated files not having the second checkbox for end at center (maybe that one is 2019).

I occasionally still see improper display on threadmill and post to check the code.

Share this post


Link to post
Share on other sites
31 minutes ago, jlw™ said:

One was the displayed toolpath is incorrect but posted correctly

That wasn't the case here, the code output exactly what the display showed. I think it may have always been like this.

Share this post


Link to post
Share on other sites

yeah buddy, lie to it and tell it one tooth. I also always drive it off a point rather than an arc. Dont know why, guess I just like to define my major diameter, just how I do it... I hardly ever use a tap anymore.... Crappy thing is sometimes you change something and it defaults back to 3 teeth...err always back plot a thread mill before posting..

  • Like 1

Share this post


Link to post
Share on other sites
8 hours ago, motor-vater said:

err always back plot a thread mill before posting..

That right there.  I ALWAYS check my threadmills in cimco backplot before taking it out or putting it on the server.

Share this post


Link to post
Share on other sites

Yes, this is what it's supposed to be doing.

The cut pattern page reads the tool data to determine how many threads are active, which is defined by the thread pitch and cut depth:

 image.png.ead96449f051ab3572fc46930b87cc17.png = image.png.9346c6d20ce65536b7fe6bb0846d7ee4.png

If you change tools or even click on your tool again, it will reinitialize that Cut Parameter page setting.

If you never take advantage of using a multi-point threadmill, I would suggest that you define your tool with the cutting length set to one tooth (in my example above, that would be .05 or 1/20). 

 

9 hours ago, motor-vater said:

I also always drive it off a point rather than an arc. Dont know why, guess I just like to define my major diameter, just how I do it...

Check out 2020 then:

image.png.11f087c14a9077f18cfdaad7cc9549f8.png

  • Like 3

Share this post


Link to post
Share on other sites

I have always wanted the ability to lock the active teeth setting or disassociate it from the tools cut length

I've had cases where editing the tool's feed rate, rpm or tool number has reinitialized

that setting and resulted in a bad toothpath

Just reselecting the tool will reinitialize this setting as well.

In So Not a Guru's example the only way to ensure this doesn't happen it to lie

when building the tool and define the tool as a single point thread mill even though it's real

length of cut is 3P

This has burned me dozens of times. I usually catch it before posting, but it has really bit me more than once

Share this post


Link to post
Share on other sites
37 minutes ago, Aaron Eberhard - CNC Software said:

Check out 2020 then:

Nice!

Share this post


Link to post
Share on other sites
2 hours ago, gcode said:

I have always wanted the ability to lock the active teeth setting or disassociate it from the tools cut length

I've had cases where editing the tool's feed rate, rpm or tool number has reinitialized 

that setting and resulted in a bad toothpath

Just reselecting the tool will reinitialize this setting as well. 

In So Not a Guru's example the only way to ensure this doesn't happen it to lie

when building the tool and define the tool as a single point thread mill even though it's real

length of cut is 3P 

This has burned me dozens of times. I usually catch it before posting, but it has really bit me more than once 

Yeah, it's the classic "I want it to be smart enough to look at the tool!"  "I don't want it to look at the tool anymore!"  dichotomy that we always seem to run into.  

In ideal-land, we would always be able to instance darn near everything from the tool & material information.  In reality-land, there's plenty of places where you want to override it.  

The problem that we have in an instance like this is we can detect if you've changed it and never change it again, but what happens when you select a completely different tool.  Would you have wanted it to update in that case?  Yeah, probably.  What about in the case where you've saved it with a value, but you're importing the toolpath and re-selecting geometry and tool?    Etc., etc., etc..   So to be predictable, if you reinitialize the tool at all (re-selecting it, changing parameters, etc.), then update the settings.

It's one of those fun no-win scenarios :)

  • Like 2

Share this post


Link to post
Share on other sites

This is one of those moments when the best enhancement would likely best be a warning that tells you that you have just changed following parameters as a result of clicking the tool, or make it a setting that we can change based on preference.  But certainly a no win situation as we all have different schools of thought on the subject.  

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