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:

help with a VERY deep pocket


cherokeechief79
 Share

Recommended Posts

ive got a square pocket to put in a part im making.

it is .438 square and about 4 inches down right against a vertical wall in 316 stainless.

It has a .4 hole through the center so theres not much coming out but the corner rad is .125 so I can only use a .25 endmill that is 6 in long.

the pocket is actually only cutting about .7 deep and needs a square corner so I cant broach it.

im cutting it now by spiraling down about .01 per pass and its working but tapering about .01.

ive made the corners about 135 in mc so it can contour even though its very little.

any ideas?

 

 

 

  • Like 1
Link to comment
Share on other sites
52 minutes ago, cherokeechief79 said:

ive got a square pocket to put in a part im making.

it is .438 square and about 4 inches down right against a vertical wall in 316 stainless.

It has a .4 hole through the center so theres not much coming out but the corner rad is .125 so I can only use a .25 endmill that is 6 in long.

the pocket is actually only cutting about .7 deep and needs a square corner so I cant broach it.

im cutting it now by spiraling down about .01 per pass and its working but tapering about .01.

ive made the corners about 135 in mc so it can contour even though its very little.

any ideas?

 

 

 

Try plunge milling it stepping over a little bit at a time?

  • Like 1
Link to comment
Share on other sites
51 minutes ago, cherokeechief79 said:

I tried that ….it walked all over the place.the square hole looked like gumbys head!

we had great success on the setup pc which was aluminum.

 

Then look to a dynamic process using the full flute of the endmill using a very small stpe over and slow speed and feed. Maybe 1000 rpm and .0005 to .001 per tooth feed rate stepping in .005 per pass.

You said there is a .4 hole thru on the next part try drilling out the corners 1st then coming back and putting in the .400 hole is possible. Might be work hardening the material with the .400 hole. I suspect your going to have to have this Plunge EDM if the tolerance tight. Let me guess it was quoted to be done in 30 seconds and one endmill was going to last 1 million parts and the management is wondering why you can't make that happen?

  • Like 2
  • Haha 2
Link to comment
Share on other sites

drilling the corners wont work because its a flatbottom and .125 rad corners doesn't leave much left in a .438 square.

leaves just a stalk in the center which would be just as much of a nightmare.

we tried dynamic but even .0005 or less it would scream.

the pocket is +- .01 but its really just - .01 because its right against a wall and cannot go bigger.

sending them out for edm is out of the question right now.

Link to comment
Share on other sites

we have a wire edm but not a sinker.

it cant be done with the wire because there is a round in the center of the square and it also does not go through the part completely.

I wish I could share a model but I cant.

im getting it done this way but its just in the tolerance.

I was just wondering if any of you encountered something similar...…….now back to tapping the 4 mm holes deeper in the same part.another nitemare as they are way too deep to threadmill!)

Link to comment
Share on other sites
26 minutes ago, cherokeechief79 said:

we have a wire edm but not a sinker.

it cant be done with the wire because there is a round in the center of the square and it also does not go through the part completely.

I wish I could share a model but I cant.

im getting it done this way but its just in the tolerance.

I was just wondering if any of you encountered something similar...…….now back to tapping the 4 mm holes deeper in the same part.another nitemare as they are way too deep to threadmill!)

Sounds like you doing the impossible so just keep doing what you can to make the impossbile happen is all I can say.

Link to comment
Share on other sites

On a similar part (but nowhere near as nightmarish), I've drilled the center, then used the Contour toolpath set to Oscillate with small High Speed bump at the bottom.  It helped dampen the harmonics/deflection of just doing the cut normally.   Then you do another contour and offset the start point by half of the High Speed distance and a smaller depth to clean up most of the material.  Kinding giving the benefits of plunge cutting without just he vertical chatter issues.

Another trick I saw once (but I've never done!) was to use a single-point tool holder and shim the tool above/behind the tool so that the tool was intentionally out of round by the amount of deflection.  But if you can't get a tool holder down there to have less than an inch of stickout, that isn't going to help you.

But yeah, to answer the question properly, EDM :)

Link to comment
Share on other sites
29 minutes ago, 5th Axis CGI said:

I was thinking of something along the same lines. Thanks for letting us know that is working for you. :thumbsup:

I'm using the Slater Tools system & broach....they were extremely helpful.  Working on a Mazak HCN-4000

Link to comment
Share on other sites

If you are determined to do this without and EDM I would drill it and flat bottom drill it to within 0.01" of the bottom (about 10mm dia). Then go in with the biggest end mill and pocket it and keep stepping down with your end mill sizes (3/8", 5/16" etc). When you get to the 1/4" long end mill set your stepovers to 0.001".  You will need to really look at the backplot carefully to check the overlap. It is in the corners that it will engage more material. 

Link to comment
Share on other sites
Quote

im cutting it now by spiraling down about .01 per pass and its working but tapering about .01.

ive made the corners about 135 in mc so it can contour even though its very little.

Are you adjusting the feedrate for the tight arc motion?  When swinging a tight arc, the OD of the tool is feeding around the arc at a much higher speed than the center of the tool.  You may have programmed .0008" FPT, but swinging a really small arc will cause the OD of the tool to experience a much higher FPT (maybe up to .002"!!!)

  • Like 1
Link to comment
Share on other sites
15 hours ago, cherokeechief79 said:

drilling the corners wont work because its a flatbottom and .125 rad corners doesn't leave much left in a .438 square.

leaves just a stalk in the center which would be just as much of a nightmare.

we tried dynamic but even .0005 or less it would scream.

the pocket is +- .01 but its really just - .01 because its right against a wall and cannot go bigger.

sending them out for edm is out of the question right now.

Why no corner drill with the Flat Bottom? Just get a .250 Flat Bottom Drill from Harvey. I've held .001 with these tools. Just leave about 0.002 for finish.

Speaking of Harvey, they have these tools with reach up to 20xD!

http://www.harveytool.com/prod/Square-Miniature-End-Mills/Miniature-End-Mills/Browse-Our-Products_255/Miniature-End-Mills---Square---Long-Reach--Stub-Flute_92.aspx

 

Nachi America has a fantastic Aqua Drill which could work. 120mm OAL, .250 diameter, 6mm shank. (You'd have about 0.720 to grip on...) Aqua EX Flat Long Shank. Series L9819.

EDP: 1489290.

http://www.nachiamerica.com/p-3/Cutting-Tools/Drills/AQUA-DRILL-EX-FLAT-OIL-HOLE-SERIES

 

  • 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...