Recommended Posts

When I try to make a thread mill program using a multi-tooth inserted thread mill cutter (https://www.secotools.com/article/p_02546918?section=products)  using bottom to top method with multiple axial depth of cut,  the tool moves directly to final depth and then moves to 2nd step. Refer attached video for more details.

If there is a solution already, please comment.

Share this post


Link to post
Share on other sites

I have ran into this before.  It can be related to either number of teeth, or if INC vs ABS or both used in your Top of Stock and Depth settings.  If you can show us those, I think we can help you better.  But hopefully this gives you a place to start.

 

Brent

Share this post


Link to post
Share on other sites

You could just set the number of teeth to 1 and let it spin up completely which would of course increase your cycle time.

It will always start how you tell it... if you pick bottom to top it will start at the bottom and step up. Choose top down and it starts at the top.

Share this post


Link to post
Share on other sites

Change to one tooth and it will cut from top to bottom on one pass or take the full depth of cut and come up with a total number of teeth needed. Divide that by two and it should be less that what your defining. Let says the hole is 40mm deep and you have a tool that gives you 30mm of teeth depth then I would except to see this. Noe change the number of teeth to give you only 20mm or maybe a little more than one tooth. Take a pitch is 1.75mm and do a little math. I came up with 11.4 teeth needed so I would tell Mastercam in the threading parameters I had 12 teeth and see if that gives me what I am looking for. With the 30mm depth tool and 1.75 mm pitch you would have 17.14 teeth and I would tell it I had 17 teeth to cut the thread. I didn't look up the tool or anything I am just using the numbers to give you an explanation that hopefully give you how I would approach this issue to solve it. Might have to adjust the number of teeth to get what your after.

HTH(Hope that Helps)

Welcome to the Mastercam forum. Have a good day, 😀

Share this post


Link to post
Share on other sites

poke poke... heh

Share this post


Link to post
Share on other sites

I agree.. the toolpath is logically incorrect and as far as I know, there is no way to make it

step down from top to bottom while still climb cutting a right hand thread.

It has been that was for as long as I can remember.

If someone knows a solution please post it

 

Share this post


Link to post
Share on other sites

Left hand cut threadmill

Share this post


Link to post
Share on other sites
1 hour ago, Rstewart said:

Left hand cut threadmill

Allied machine threadmills are left hand cut. We cut from top to bottom using g42 which is climb milling

Share this post


Link to post
Share on other sites
24 minutes ago, Leon82 said:

Allied machine threadmills

Carmex makes these and calles them Hardcut.. they work really well for threadmilling super alloys

I believe Carmex had a patent on them, which has now expired

I didn't know Allied Machine built them now, but Harvey Tools has an extensive line of these tools in smaller sizes

A Pro Tip, when you first introduce these tools to the floor, put a piece of masking tape over the M03 button on the control

The operator is sure to screw it up a couple of times.. muscle memory  is a powerful thing.

It doesn't wreck your part but it strips all the teeth off the left hand thread mill

 

  • Like 1

Share this post


Link to post
Share on other sites

Yea, sometimes Mastercam switches the direction on us.

 

Camplete posts an error about spindle speed when is sees the m4 so we use that to know we have the correct direction

Share this post


Link to post
Share on other sites

We buy Johs Boss and some Walter threadmills. The Johs Boss threadmills all specify convention mill top down for all of their threadmills. Some walter threadmills suggest it as well as do 1 cut up and 1 cut down for tough stuff.

Its been a few a years since i have bought a climb cutting threadmill. The fun threadmill from Walter has 3 rings of teeth spaced 1" apart on the tool shank. I love handing that threadmill to a new guy and tell him to make me a 2"-8 un thread 3" deep in 1 pass :)

Share this post


Link to post
Share on other sites
22 hours ago, crazy^millman said:

Change to one tooth and it will cut from top to bottom on one pass or take the full depth of cut and come up with a total number of teeth needed. Divide that by two and it should be less that what your defining. Let says the hole is 40mm deep and you have a tool that gives you 30mm of teeth depth then I would except to see this. Noe change the number of teeth to give you only 20mm or maybe a little more than one tooth. Take a pitch is 1.75mm and do a little math. I came up with 11.4 teeth needed so I would tell Mastercam in the threading parameters I had 12 teeth and see if that gives me what I am looking for. With the 30mm depth tool and 1.75 mm pitch you would have 17.14 teeth and I would tell it I had 17 teeth to cut the thread. I didn't look up the tool or anything I am just using the numbers to give you an explanation that hopefully give you how I would approach this issue to solve it. Might have to adjust the number of teeth to get what your after.

HTH(Hope that Helps)

Welcome to the Mastercam forum. Have a good day, 😀

As the total insert length is 40mm, hence it is not recommended to engage the full length of the insert at once. As per the tool specification, the TM cutter can produce 65mm depth whereas the insert length is 40mm. If I put 65mm as final depth in the program, then the tool moves to the final depth at the first pass will damage the tool. 

Share this post


Link to post
Share on other sites

You will have to make 2 ops with a depth difference equal to a multiple of the pitch

Share this post


Link to post
Share on other sites

Seems the simplest solution is run it as a conventional cut with G42...

That said, all insertable threadmills I have seen have plenty of neck clearance to cut bottom to top

Share this post


Link to post
Share on other sites
5 hours ago, Debaprakash Nayak said:

As the total insert length is 40mm, hence it is not recommended to engage the full length of the insert at once. As per the tool specification, the TM cutter can produce 65mm depth whereas the insert length is 40mm. If I put 65mm as final depth in the program, then the tool moves to the final depth at the first pass will damage the tool. 

Exactly so you put 20mm and tell Mastercam top to bottom to get the job done. OR

4 hours ago, JParis said:

Seems the simplest solution is run it as a conventional cut with G42...

That said, all insertable threadmills I have seen have plenty of neck clearance to cut bottom to top

Grind a relief on the tool so you can use it like being mentioned. I have thread milled for 25+ years and never had a problem machining from top to bottom or bottom to top with a tool designed to do it. Each situation presents it’s own issues to over come and that is part of our role as machinists and programmers to overcome them. Great discussion and hopefully you and others have glemmed good information from this thread. 

Share this post


Link to post
Share on other sites

whenever i have had to do this i use multi-pass, just making sure the depth is less than the thread pitch so it doesnt ram into the shank. then just use bottom to top.

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