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:

thread milling question


Recommended Posts

gonna be milling some 6mm standard threads in hardened s-7. using a solid carbide cutter. only thing different is the cutter says to run with a M04 instead of M03 in the nc code. do I need to change anything in my thread mill path besides the way the cutter turns. Currently I conventional cut and I start at top and go to bottom with my thread mill cutters but this a first with one that has to be run cutting in reverse or M04 spindle code. just looking for any info that any one has that may have run these types of cutters before when doing thread milling. thanks in advance.

Link to comment
Share on other sites

its internal threading and I have always done my threadmilling from top to bottom. Is this the wrong way of doing so because it works with no problems. as far as the m04 code for these particular cutters I was thinking just make sure and go ccw with spindle and to climb cut instead of conventional from top down..and thanks fo rthe info but please correct me if im wrong about normal thread mill cutters(m03) spindle rotation and weather starting from top to bottom versus bottom to top.I have only done about 25 to 50 holes using the thread mill path and had great success with right hand threads starting at top to bottom but never tan across using a M04 rotation cutter for right hand internal threads..also Im not sittting in front of my work computer it may default to bottom to top when climb cutting with a cutter spinning in reverse (M04) to produce right hand threads..for threads im new to I always do a test run in a scrap piece of alumunium before I cut them in the actual part so as to not scrap the part for im still learning the thread milling ans so far I like it just want to make sure I do it right.. thanks..

Link to comment
Share on other sites

I always run my threadmills from the bottom to the top. It does not mean much for thru holes but I sure don't want to be doing that on blind holes, as there may be chips on the bottom of the hole.

IMO, it's a good habit to be threadmilling from the bottom to the top.

  • Like 1
Link to comment
Share on other sites
Threadmills are no different than end mills. They have ground teeth with clearance behind the cutting edge and only cut in one direction. Just as you cannot spin an end mill in the opposite direction to change a convention cut into a climb milling cut.

 

True. What we're talking about is that some threadmills are ground for CCW rotation, which makes a climb cut go top down on a right hand thread.

Link to comment
Share on other sites

I would recommend checking out Carmex Hardcut Left hand cut Use M04 Climbmills top to bottom, Great for Deep, and Blind holes and hard Material, this code is running as we speak and 1 tool has done 300 plus Holes

Class 3 .25 min thread 304 Stainless 15sec per hole

 

N8T8M6S9100(8-32 THREAD MILL)

Y_[1]=$TC_DP6[$TC_MPP6[9998,1],1]*1

IF(Y_[1]>.07)GOTO N5555

IF(Y_[1]<.05)GOTO N5555

(TOTAL DEPTH= Z-.28)

M50(THREADMILL 8-32 HOLES AT G54)

G43G54X-1.031Y-.8121Z.1H8T9M4

G1Z.028F40.

G1G42D8X-.949Y-.8121

G2X-.949Y-.8121Z-0.0033I-.082

Z-.0346I-.082

Z-.0659I-.082

Z-.0972I-.082

Z-.1285I-.082

Z-.1598I-.082

Z-.1911I-.082

Z-.2224I-.082

Z-.2537I-.082

Z-.285I-.082

G1G40X-1.031Y-.8121

G0Z.2

  • Like 1
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...