Project of the Month built by Johno1958

Help Support Home Model Engine Machinist by donating using the link above or becoming a Supporting Member.
Home Model Engine Machinist > The Tools and Tips > Tips and Tricks > Milling a pocket

Thread Tools
Old 03-16-2017, 08:17 AM   #1
stragenmitsuko's Avatar
Join Date: Jan 2016
Posts: 114
Liked 48 Times on 29 Posts
Likes Given: 7

Default Milling a pocket

I seem to have a minor problem when milling a pocket , or better a corner .

This is a pretty deep pocket, 58mm ( 2 1/4 ") and I'm using a very long 10mm
endmill . I need to use that small diam endmill , cause later on the part will be reversed and the rounded corner removed .

I make a U shaped cut , conventional milling . After each pass , the cutter is lowered or better the table is raised 5mm for a next pass .
This is a casting so I'm only cleaning up the edges . Abt 3 mm (1/8" ) to remove from the sides . It varies cause my casting isn't perfect .
In the corner the cutter seems to flex , an instead of having a nicely chamefered corner I'm getting something that looks overcut .
The part is good and fuctional , but I just don't like the look of it .

If this was solid material being carved out , I would drill the corners first 0.5 mm from the edge and then mill it . Then I don't have this problem .
But as this is a casting that won't work .

Any tips or tricks to avoid this .


Attached Thumbnails
IMG_0004.JPG   IMG_0005.JPG  
stragenmitsuko is offline  
Reply With Quote
Old 03-16-2017, 09:01 AM   #2
Nick Hulme
Join Date: Oct 2008
Posts: 283
Liked 67 Times on 50 Posts
Likes Given: 32


You can peck plunge cut your corners with a centre cutting end mill.
Direction of cut changes how the cutter pulls at the corners and reduced contact, i.e. shallower cuts, will reduce cutter deviation.
You can use a cutter with much shorter flutes if you reduce the shank by a few thou from the end of the flutes to the cut depth.
If you're not already using carbide it might be worth trying for it's increased rigidity and single flute end mills are great for profile cuts in aluminium.
If you're not already use air or flood to clear chips.

- Nick

W.C. Fields said "You can't cheat an honest man", he should have followed that with "But, you can always find a credulous fool if you need one"
Nick Hulme is offline  
Reply With Quote
Old 03-16-2017, 09:53 AM   #3
Project of the Month Winner!!!
Jasonb's Avatar
Join Date: Mar 2008
Location: Surrey, UK
Posts: 2,254
Liked 424 Times on 266 Posts
Likes Given: 18


I'd take less of a cut say 2.5mm deep per pass so the cutter will not be removing as much material and therefore won't deflect as much.

Also cut the pocket say 0.2mm under size then go back and cut to finished size which could be done in 5mm steps.

This one is also 10mm cutter, 52mm deep. I bored out first then just went round and round teh edges size of cuts as above. Dab of parafin and a sharp cutter



And what the inside finish came up like

Jasonb is offline  
People Like This 
Reply With Quote
Old 03-18-2017, 12:56 PM   #4
Join Date: Aug 2011
Location: Berea OH.
Posts: 369
Liked 42 Times on 40 Posts
Likes Given: 191


Drill the corners 1st staying perhaps .010" away from your finish dim and staying off the bottom. use a flat bottom drill (easily ground) to finish the bottom.
Rough the pocket, Then plunge corners to finish with the end mill. then finish the pocket with the end mill.
purpleknif is offline  
Reply With Quote
Old 05-25-2017, 10:48 PM   #5
Join Date: Jan 2010
Posts: 48
Liked 4 Times on 4 Posts
Likes Given: 7


Is your endmill center cutting? I had similar problems til I realized the long cutter I had was not center cutting.
Mill with a regular length cutter ,switch to the long one. Make sure the long cutter reaches the bottom of the slot in one pass. Looking at the pic the cutter may not be center cutting. Not positive from the pics.
kwoodhands is offline  
Reply With Quote
Old 05-26-2017, 11:55 AM   #6
Senior Member
ShopShoe's Avatar
Join Date: Oct 2010
Location: Central Iowa, Central U.S.A.
Posts: 759
Liked 119 Times on 108 Posts


Perhaps a roughing cutter first, then clean it up.

ShopShoe is offline  
Reply With Quote
Old 05-26-2017, 02:09 PM   #7
Project of the Month Winner!!!
gbritnell's Avatar
Join Date: Jul 2007
Posts: 2,526
Liked 545 Times on 526 Posts


While coventional milling has it's place cutting into a corner isn't one of them. As has been mentioned I would plunge the corners out, staying away from the finished number and working my way in. Once you have the corners where you want them climb cut the walls going into the corner. This way the cutter will want to climb away from the corner rather than pulling itself into it.

Talent unshared is talent wasted.
gbritnell is offline  
Reply With Quote

Thread Tools

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
pocket nc 5-axis petertha CNC Machines and Conversions 2 06-29-2015 12:18 PM
Pocket V8 Sixtysixdeuce A Work In Progress 3 06-16-2014 06:12 AM
CNC deep pocket aluminium milling laurent_parti CNC Machines and Conversions 6 08-02-2013 11:00 AM
pocket scriber lectrician Tips and Tricks 6 06-23-2011 11:14 PM
How to mill a bowl pocket milotrain General Engine Discussion 21 03-07-2011 08:17 AM

Newest Threads

- Top - Member List