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:

Never Thread Milled Before


tiredtoolmaker
 Share

Recommended Posts

I'm pretty much in the dark here. I searched the archives but didn't find much.

I'm using X7, what are my options on importing or creating thread mills? When I try to create a new tool, there is no thread mill tool type.

Do I use undefined tool and somehow create the geometry? Do I draw the tool and import it?

Any suggestions are greatly appreciated...

:unsure:

Link to comment
Share on other sites

In X7 if you want to see the thread in verify, create it as a custom tool

There is a BUNCH of info around on creating custom tools if you do not know how

 

This should help on defining custom tools

 

Edited by Guest
Link to comment
Share on other sites

If you don't care about seeing the actual thread in verify just call it an endmill with the correct diameter. Use your thread mill tool path as usual. The only thing you will be lacking is the thread shape in verify. It will look like a hole instead.

Link to comment
Share on other sites

Typically, when you first generate the Thread Mill path, it will cut an undersized thread. You can use CRC on the machine to adjust the thread size, or you can use the "Overcut" parameter in the Thread Mill Tool Path, to increase the size of the helical arcs generated in the NC Code. Depending on the thread size, I've up in up to .006 in the Overcut parameter, to get the correctly sized threaded hole...

Link to comment
Share on other sites

I program everything to the number and let cutter comp do it's job.

I have been burnt recently by Carmex and Iscar with threadmills.  Be sure on the first one to comp the tool big and sneak up on it.  Use the same threadmills for consistency.

  • Like 2
Link to comment
Share on other sites
46 minutes ago, Matthew Hajicek™ - Conventus said:

I've been complained to when the floor setup a different brand of threadmill with a different cut diameter.  Boss saved a few bucks on them and scrapped a few parts.

Them: Your program scrapped that threadmilled hole.

Me: How did that happen? Was the tool taught properly? (as I'm looking at the tool they setup and find it to be different than the one called out)...This is the wrong tool!

Them: It's the only threadmill I found...

Me: What about these? (as I show them the tools I called out still in the box they came in WITH the job # on them)

Them: Oh. Didn't know we had them...

Me: :wallbash:

  • Like 4
Link to comment
Share on other sites

I've been single point threadmilling for years. I just started buying multi point threadmills last year. Does seem to cut smaller than programmed thread size either way.

I've pulled a part out of the chuck threadmilling with the multi point long ones. Seems to be an inordinate amount of tool pressure.

Even though I do it a few times a month whenever you can tap it is so much faster. Through holes on 3/4 or less I usually tap with OSG Hy-pro.

Anything tapered (pipe fittings) I thread mill.

Once you do it a couple times all fear goes away.

You can get cheap multi flute 2 sided 60 degree chamfer tools that work just fine for thread milling. Trust me LOL.

Link to comment
Share on other sites
2 hours ago, jlw™ said:

Tom, forgive me.  I'm having trouble wrapping my head around climb cutting top down on a right hand thread.  Send me a file?

I'm not at my PC right now. I'll get you a file in the AM

Picture this

Left hand tool...CCW is climb cutting

The toolpath is CW from the top spiraling down

CDC is G42

In Mastercam it's dead simple 

Define the tool as single point G04

Set thread mill for right hand thread top to bottom

MC does the rest

Carmex  has an excellent app for selecting the right tool and feeds and speeds

Be sure to post the code in the app as it calculates the correct feed rate comped

for the hole size

 

 

Link to comment
Share on other sites

Here is a sample toolpath that we ran on our Okuma MU10000 5X mill

The alloy was 15-PH per H1025 ...  not too bad, but the part was  much too expensive to be poking with taps

Here is a link to Carmex's thread milling app.

You can run it directly from this link or down load and install it for offline use

Carmex Catalog

Use the Tool recommendation and Programming tab.

It will walk you through choosing a tool, recommend radial stepover, give you feeds and speeds and generate an NC file

I don't use the code, but I do generate the code to get the correct feed rate

 

hardcut.zip

Link to comment
Share on other sites

I program from the minor dia because i use entity and the threads are modeled as the minor. I use the over cut with the tap pitch as a value. I usually back it off .003 and tune it with cutter comp.

A couple of my coworkers use point so they put the major dia in. But then they ask me the major of some still thread and I have no idea so they have to go looking for that info.

Link to comment
Share on other sites
3 hours ago, F10Brandon said:

I want to give this a go one day, seems like a much safer process then a tap. Although I use Emuge multi-taps and they are pretty good.

Two things on one part required theadmilling.

#1 over 1000 hours of run time and a $50k forging to start.

#2 HST Spindle with no ability to sync tap.

I was thread milling back in 91 on a Fadal. We had to do a NPT and one of tool vendors made the NC code to run on the machine. Done all types of threads since then and every time it really just comes down to the right tool with the correct speeds and feeds. Once you have it dialed in you can do just about anything.

  • Like 2
Link to comment
Share on other sites
On 6/30/2017 at 4:05 PM, Matthew Hajicek™ - Conventus said:

Boss saved a few bucks on them and scrapped a few parts.

Sounds to me like the boss bent down to pick up a penny and a dollar fell out of his pocket.

  • Like 2
Link to comment
Share on other sites
18 hours ago, SlaveCam said:

PLEASE don't take this as an insult but a "tool maker" and "never threadmilled" just do not fit ;) I always thread mill using control compensation, never trust the threadmills..

How about "Old Fashioned Tool Maker". Until a few of years ago, it was all manual equipment. Horizontal and vertical mills, shapers, Troyke rotaries, surface grinders, ID and OD grinders and lots of granite plates. I been with same company 40 years and as long as job got done they didn't care how. We are strictly a support shop so we are not in the competition arena.

Link to comment
Share on other sites
On 7/4/2017 at 6:37 AM, Leon82 said:

I program from the minor dia because i use entity and the threads are modeled as the minor. I use the over cut with the tap pitch as a value. I usually back it off .003 and tune it with cutter comp.

A couple of my coworkers use point so they put the major dia in. But then they ask me the major of some still thread and I have no idea so they have to go looking for that info.

Keep a chart handy:

http://web.archive.org/web/20160430015806/https://www.physics.ncsu.edu/pearl/Tap_Drill_Chart.html

 

Link to comment
Share on other sites

Make sure and use this formula for your chipload and save yourself A LOT of headaches.

ipt (holedia - cutterdia) / holedia

 

When you have to put a 2 1/2-4 thread 2 inches deep in a solid block of unknown steel that is 68HRC, thread milling is a better than burning 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...