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:

figure chip thinning


Recommended Posts

I run alot of 1/2" carbide endmills in 1018. My question is what is the formula for figuring out chip thinning. Say my endmill specs 475 sfm and is 4 flute and recommends .003 to .005 per tooth. Now that is running it the standard way not high speed machining. Usually I like to cut full length of flutes, or full depth of pocket at 10 percent dia. of cutter. But I am always guessing on the speed and feed. So is there a formula for chip thinning? Thanks in advance.

  • Like 2
Link to comment
Share on other sites

What I came up a while ago in excell....

 

 

=(.5(Tool Dia/WOC))/SQRT((Tool Dia/WOC)-1)*desired chip thickness

 

(WOC = width of cut, so at 10% stepover with a .5 tool is = to .05)

 

so to work it out...

 

.5(.500/.05) = 5

 

sqrt ((.500/.05)-1) = 3

 

say you want a .003 chip

 

(5/3)*.003=.005

 

so you program for .005/tooth

  • Like 1
Link to comment
Share on other sites
=(.5(Tool Dia/WOC))/SQRT((Tool Dia/WOC)-1)*desired chip thickness

 

The formula works well on calculator, but not in Excel ... Try this one instead:

 

=(.5*(Tool Dia/WOC))/SQRT((Tool Dia/WOC)-1)*desired chip thickness

 

For me, it looks like this:

 

=(0.5*(O7/O8))/SQRT((O7/O8)-1)*O9

 

O7 = Tool Dia

O8 = WOC

O9 = desired chip thickness

 

HTH

  • Like 1
Link to comment
Share on other sites

Thank you all for you help. I milled some 1018 today 1.25" depth of cut and a .05 step over with a rpm of 4600 and a feed rate of 225 ipm with no problem at all. I did 20 parts and the endmill didnt even look like it was used. I also ran it dry. And this was a on a 10hp power spindle on a fadal. So I just can imagine what a real machine could do. I really think I can go alot faster yet its just a matter of the endmill now. Again thank you all for the help.

Link to comment
Share on other sites
  • 10 months later...

I found a few more calculators for those that may still be looking.

 

http://integrexmachi...0Calculator.PDF

 

http://twitpic.com/5m7gdv For this link, select the URL to download: http://tinyurl.com/3u4kl5u

 

Calculators of all types for the trade:

 

 

http://www.ipstooling.com/resources.swf

 

 

Still trying to wrap your head around the Chip Thinning theory? This may help.

 

http://www.volumill....ite_Paper_1.pdf

  • Like 1
Link to comment
Share on other sites
  • 4 months later...
  • 6 months later...
  • 3 months later...
  • 2 months later...

I like the formulas that y'all have provided, but I have a couple of "?'s"...

 

First, does step over and step down work the same in calculating chip thinning? (ie: helix boring a .094" hole with a .0625 4FL EM with a .002 RGH Pitch)

 

Second, does it change even more if one were using a .01 corner radius on the 1/16" EM?

 

Lastly, how would one go about calculating such variables???

 

Sorry, not trying to thread jack, just trying to expand on the whole "Chip Thinning" information.

 

 

Thanks

  • Like 1
Link to comment
Share on other sites
  • 3 weeks later...

When helical boring chip is actually thickening.

People who do a lot of thread milling know that.

Its caused by the difference in programmed feedrate of the center of the tool and the actual circumference of the tool when interpolatimg tight internal radiuses.

 

When milling outside radiuses the chipload actually is going down.

 

But still when radial engagement is low enough you will get see chip thinning even when milling ID.

 

Now if your endmill has a radius and depth of cut is smaller that that you also add axial chip thinning to the mix.

 

So when doing helical milling you can have up to 3 chip thinning/thickening formulas apply at the same time. Calcs like HSMAdvisor can compensate for all of them.

 

 

  • Like 1
Link to comment
Share on other sites
  • 3 weeks later...

Thanks for the advice. I've now downloaded the HSM Adivisor and I'm going to play with it some. The little bit that I've looked at it since download looks very interesting. I wish I knew more of the mathematics behind the formulas they are using to calculate their data so I could further understand the entire process. But, I'm sure I'll get by with solutions provided for now. :)

  • Like 3
Link to comment
Share on other sites
  • 6 months later...
  • 5 weeks later...

I like the FSWizard, nice interface. I really like the GWizard by Bob Warfield, Its a complete calculator. I just came into using the FSWizard; its missing a few things like tapping and when turning the GWizard mini-calc does a little more.

 

-Bill

FSWizard is free. I have not updated it in over 6 months.

Been busy developing HSMAdvisor for PC and FSWizard for mobile devices.

I now have both iphone and android versions.

And yeah, they both now do tapping as well.

Also you can integrate HSMAdvisor with Mastercam to some degree.

This will save a lot of time as well.

  • Like 1
Link to comment
Share on other sites

Also you can integrate HSMAdvisor with Mastercam to some degree.

This will save a lot of time as well.

 

Care to elaborate on this? Do you have access to the SDK I am thinking it would be cool to make a tab that sits in the operation manager that works. One click update speed and feeds to operation would be a sweet addition. I might can get you some assistance with that if you are up to the challenge.

  • Like 2
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

×   Your link has been automatically embedded.   Display as a link instead

 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

×