rgollar

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

Share this post


Link to post
Share on other sites

I thik there is an Iscar Chip thinning calculator you can D/L. Just Google it.

  • Like 1

Share this post


Link to post
Share on other sites

Check out the Iscar Quick Calculator on the forum FTP.

I checked what you posted and to maintain a .005 chipload with chip thinning on that tool the adjusted chip load would be .0063 FPT.

Which gives you a spindle speed of 3629 and 91 IPM feed.

Share this post


Link to post
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

Share this post


Link to post
Share on other sites

Thank you JMC thats what I was looking for to see how it was broken down. Much appreciated

Share this post


Link to post
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

Share this post


Link to post
Share on other sites

There is this way...

 

Load X5, choose a 2D Highspeed Dynamic mill toolpath. Select an Iscar HEM tool out of the Iscar HEM tool catalog, click the HEM button, slide slider over to the max your machine can handle and post.

Share this post


Link to post
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.

Share this post


Link to post
Share on other sites

Nice! Feel free to share your data in the dynamic milling database. Link to the entry form and results in my sig. It's also got a mmr calculator, if that's any incentive. :rolleyes:

  • Like 1

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
Share on other sites

I know this is an older thread, but I found THIS online calculator for chip thinning.

FSWizard

 

pretty easy to use, and no guesswork

  • Like 2

Share this post


Link to post
Share on other sites

For all the iPhone users out there...

 

go to the app store and look for iMachinist. It includes some pretty handy calculators for radial chip thinning and high feed optimization for button inserts

Share this post


Link to post
Share on other sites

For all the iPhone users out there...

 

go to the app store and look for iMachinist. It includes some pretty handy calculators for radial chip thinning and high feed optimization for button inserts

 

This app was built by our very own Evil Machinist!

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
Share on other sites

Look at the Toroid Calculator here, http://dapra.com/tech/calculators.htm

 

This calculator shows for inserted tools but I am not sure why one could not use it for solid tools with different corner configurations.

I would not reflect proper metal removal rates.

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
Share on other sites

I keep a ipod touch handy with the journeyman machinist app.

I think it was 10 bucks ,Very handy features!

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
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

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