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:

Threadmill Operation Bug? WIerd quirk


Metallic
 Share

Recommended Posts

Hey all. So I just scrapped a critical part on my machine because of a crazy threadmilling quirk. Something Ive never seen happen.

I use my Harvey thread mill. I copy/paste the operation and copy/paste the tool in order to change the diameter (new tool number as well), but keep the original tool unchanged in case i need to come back to it.

BUT. Mastercam CHANGED THE PITCH back to the default 0.05 for no reason. I just recreated the issue, simply by changing to a different diameter tool, Mastercam has changed the pitch back to default 0.05. I changed no other parameters.

 

Anyone ever had this happen before? Or am I missing something?

Thanks!

correct.JPG

flip tool.JPG

Link to comment
Share on other sites

Threadmill has had some really weird stuff for a couple versions of Mastercam. 

In 2017, if you used "Incremental" for the Linking Parameters, it will treat the "Depth" as an actual 'Incremental from Geometry' value, and the Top of Stock as 'Incremental', but the Retract and Clearance values are Absolute values. So if you enter "0.25" for Retract, thinking "that will be .25 above my Geometry", nope, that's 0.25 Absolute!

  • Like 1
Link to comment
Share on other sites

This pitch bug cost me an M36 hole in a $90,000 forging and egg on my face when I had to tell a customer and then do a work-around.  At least it was an extremely high pressure hydraulic manifold that only weight about 24k lb and was 4340 forged so we couldn't weld it.

 

Since then, I find myself spending more time checking threadmill paths than making them.  Also I always take a quick look at the posted code and then calculate the pitch again to make sure posted code is correct.  I also set my pitch in my threadmill tool definitions EXACTLY.  Your defaults can also mess with this as that's where that 0.05 comes from.  My most common thread was an M36 so I set my default to that.  No way of knowing how many times that helped me but I'm sure it did at least a few.

  • Like 2
Link to comment
Share on other sites
On 5/17/2019 at 7:33 AM, jlw™ said:

This pitch bug cost me an M36 hole in a $90,000 forging and egg on my face when I had to tell a customer and then do a work-around.  At least it was an extremely high pressure hydraulic manifold that only weight about 24k lb and was 4340 forged so we couldn't weld it.

 

Since then, I find myself spending more time checking threadmill paths than making them.  Also I always take a quick look at the posted code and then calculate the pitch again to make sure posted code is correct.  I also set my pitch in my threadmill tool definitions EXACTLY.  Your defaults can also mess with this as that's where that 0.05 comes from.  My most common thread was an M36 so I set my default to that.  No way of knowing how many times that helped me but I'm sure it did at least a few.

I hate how this tool path treats pitch and the number of teeth setting

I recently sent a bad thread mill path to the floor for a very expensive part

Fortunately for me, the operator is old old school and trusts nobody

He ran my code though his calculator and called me on it.

Just changing the feed rate on a tool can change the number of teeth setting and scrap a part

 

 

Link to comment
Share on other sites
On 5/16/2019 at 6:36 PM, Metallic said:

Hey all. So I just scrapped a critical part on my machine because of a crazy threadmilling quirk. Something Ive never seen happen.

I use my Harvey thread mill. I copy/paste the operation and copy/paste the tool in order to change the diameter (new tool number as well), but keep the original tool unchanged in case i need to come back to it.

BUT. Mastercam CHANGED THE PITCH back to the default 0.05 for no reason. I just recreated the issue, simply by changing to a different diameter tool, Mastercam has changed the pitch back to default 0.05. I changed no other parameters. 

 

Anyone ever had this happen before? Or am I missing something?

 

Sorry, I just re-read this, and I don't think it's the same thing that was discussed previously.  Can you send a file into QC including which version you're experiencing this in?  I can't replicate your behavior from scratch.  I tried in 2019 & 20.

 

Here's how I did it.  I set up a Threadmill op on a Ø.500" circle, and defined a Ø.25" 24 TPI single point thread mill. 

image.png.8230265af632973dbbefaf50a70c61ea.png

I then copy/pasted the toolpath, edited the tool to increase diameter to .375" and the tool number to 2, while still leaving a 24 TPI and 1/24th as the flute length:

image.png.65dcee2a053642205f9aa38b8b5574ed.png

No matter what I do, my cut parameters don't update:

image.png.b7a169612f34271a7e4979d56cedd70b.png

What did I do wrong?

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

Sorry, I just re-read this, and I don't think it's the same thing that was discussed previously.  Can you send a file into QC including which version you're experiencing this in?  I can't replicate your behavior from scratch.  I tried in 2019 & 20.

 

Here's how I did it.  I set up a Threadmill op on a Ø.500" circle, and defined a Ø.25" 24 TPI single point thread mill. 

image.png.8230265af632973dbbefaf50a70c61ea.png

I then copy/pasted the toolpath, edited the tool to increase diameter to .375" and the tool number to 2, while still leaving a 24 TPI and 1/24th as the flute length:

image.png.65dcee2a053642205f9aa38b8b5574ed.png

No matter what I do, my cut parameters don't update:

image.png.b7a169612f34271a7e4979d56cedd70b.png

What did I do wrong?

I think they are setting the pitch in the thread mill field and not in the tool.

 

So if you click the tool it resets the field to match the tool value

Link to comment
Share on other sites

I use a lot of single-profile threadmills, so I can cut a 10-32 and a 10-24 with the same tool.  If I defined it as a 24 pitch and use it to cut a 32 pitch, then any time I change something about the tool the operations that use it will change to 24 pitch.  Similarly if I'm using a 1/4-28 multi-profile threadmill to cut a dual lead 1/4-14, touching the tool will revert it to 28 pitch.

Link to comment
Share on other sites
On 5/21/2019 at 10:14 AM, Aaron Eberhard - CNC Software said:

Sorry, I just re-read this, and I don't think it's the same thing that was discussed previously.  Can you send a file into QC including which version you're experiencing this in?  I can't replicate your behavior from scratch.  I tried in 2019 & 20.

 

Here's how I did it.  I set up a Threadmill op on a Ø.500" circle, and defined a Ø.25" 24 TPI single point thread mill. 

image.png.8230265af632973dbbefaf50a70c61ea.png

I then copy/pasted the toolpath, edited the tool to increase diameter to .375" and the tool number to 2, while still leaving a 24 TPI and 1/24th as the flute length:

image.png.65dcee2a053642205f9aa38b8b5574ed.png

No matter what I do, my cut parameters don't update:

image.png.b7a169612f34271a7e4979d56cedd70b.png

What did I do wrong?

As Leon said, I was using my "Thread Pitch" in the operation manager instead of in the tool dialogue window.

 

As a previous poster said....what if I wanted to use a single point threadmill to cut two separate thread pitches in the same program?

In mastercam 2019

 

Who should I forward this file to?

 

Wheel_Nut.ZIP

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...