Need advice on machining O-Ring groove
Close
Login to Your Account
Results 1 to 16 of 16
  1. #1
    Join Date
    Sep 2012
    Location
    Cincinnati
    Posts
    172
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    30

    Default Need advice on machining O-Ring groove

    I need to make a an o-ring groove that will capture the o-ring. In the past all the o-ring grooves I machined were for static pressure using the Parker guidelines and the o-rings move around in those grooves.

    The project is a valve cover adapter for a race head. The top of the adapter is screwed and glued to the cast aluminum valve cover and the bottom rail will have the o-ring. The o-ring will be either a .103 or .139 diameter. 6061-T6 material.

    My understanding is that the Harvey dovetail cutter is an excellent way to go. But I don't think I have a chance in hell of being successful with it but would appreciate feedback. Not sure if I looked at the .103 or .139 one, but the Harvey guideline is 28,000 rpm and 48 ips feed. Problem! My machine is only good for 4500 rpm! Any chance I can evacuate the chips at 4500 rpm so I don't break the cutter? I'm still learning my speeds and feeds so I don't know exactly what to expect.

    This is not exactly a tough sealing application so my other plan is to just machine a rectangular slot that would pinch the o-ring by a few thousandths just so it doesn't slip out. I would determine the depth by trial and error.

    Suggestions?

    Picture of a wooden prototype valve cover adapter and a link to a Harvey cutter.

    http://www.harveytool.com/ToolTechIn...olNumber=23814

    rail.jpg

  2. #2
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    6,825
    Post Thanks / Like
    Likes (Given)
    1617
    Likes (Received)
    4747

    Default

    4500 RPM is fine, just use a slower feed (and IPM, not IPS), perhaps .0008/tooth. Mill the slot to max width first, figure out where the safest entry point is for the dovetail cutter and open that up with a regular endmill.

    Chip evacuation is what you care about, at worst an air blast, better a mist setup, best a proper coolant stream. Are you doing this on a manual mill, a CNC knee mill, or ?

  3. #3
    Join Date
    Sep 2012
    Location
    Cincinnati
    Posts
    172
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    30

    Default

    Thanks! I meant IPM - IPS is a company I deal with........

    The machine is an Atrump bed mill with a Centroid control. My current coolant system is not very good. Bought the machine new around a year ago. Pretty happy with it but there are some things that just need to be a bit better like the cooling system. I bought a good external pump/tank but have not plumbed it yet. I can do that before I do the grooves.

  4. #4
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    6,825
    Post Thanks / Like
    Likes (Given)
    1617
    Likes (Received)
    4747

    Default

    Do some test cuts on a scrap of Al before committing to the actual part. My .0008/tooth is just a quick guess, you can confirm with Harvey about best feed when using limited RPM. You also want to see if you can do a center pass, then two climb finish passes of about .002" offset - I don't know if these cutters are meant for one-shot cutting.

    Be sure to have the program correct before cutting, any panic and a emergency stop will be unpleasant.

    I'd go with the larger O-ring if possible. Use some 600 sandpaper to radius the upper edge of the cut groove to ensure no burrs or sharp edges when pressing in the O-ring. Clean the groove carefully before installing the seal. Watch this during use, you don't want crap in this groove during engine work.

  5. #5
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,997
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    usually you rough out most of material with roughing cutter and a 2nd cutter just takes a light finishing cut
    .
    if nothing else you get a better finish if only cutting small amounts

  6. #6
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,242
    Post Thanks / Like
    Likes (Given)
    1803
    Likes (Received)
    798

    Default

    I use Internal Tool's oring cutters, but same thing applies: Run an endmill to remove the center, down to within 0.005 in depth, and leave a few 0.001's on each side for the dovetail to remove.

    Spin it as fast as you can, flood it with coolant, and keep your feed rate commensurate to your RPM.
    Bring on the Gravy!

    Doug.

  7. #7
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    436
    Post Thanks / Like
    Likes (Given)
    29
    Likes (Received)
    235

    Default

    AB Tools sells a fantastic form cutter for this application. I use it for engine intake/head sealing surfaces, carburetor flanges, etc. It is for 1/8" standard oring material (0.140") you can get from McMaster or wherever. Make sure you're sitting down when you look at the price of the Loktite oring adhesive if you're installing the orings.

    Oops Pierson Workholding sells this made by AB Tools. I got quotes from AB for a 1/16" Standard Oring of the same design and they were reasonable for sure.

  8. #8
    Join Date
    Jul 2010
    Location
    Joliet Il
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    30

    Default

    A dovetailed o-ring groove is probably overkill for this application; I'd just mill it with a straight endmill and then use Vaseline to hold the o-ring in place during assembly. Superglue works to hold o-rings in place also.

  9. #9
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,217
    Post Thanks / Like
    Likes (Given)
    1432
    Likes (Received)
    1514

    Default

    Quote Originally Posted by Keyepitts View Post
    A dovetailed o-ring groove is probably overkill for this application; I'd just mill it with a straight endmill and then use Vaseline to hold the o-ring in place during assembly. Superglue works to hold o-rings in place also.
    I would check the o-ring mat'l before using super glue!

  10. #10
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,217
    Post Thanks / Like
    Likes (Given)
    1432
    Likes (Received)
    1514

    Default

    Quote Originally Posted by doug925 View Post
    I use Internal Tool's oring cutters, but same thing applies: Run an endmill to remove the center, down to within 0.005 in depth, and leave a few 0.001's on each side for the dovetail to remove.

    Spin it as fast as you can, flood it with coolant, and keep your feed rate commensurate to your RPM.
    Bring on the Gravy!

    Doug.
    LoL ya if the tool doesn't break AND you have quoted appropriately. We did a few pieces that had some curvy geo for an o-ring (or some gasket), freekin' took forever to cut! Think it was a toolsteel or 4140ph....

  11. Likes doug925 liked this post
  12. #11
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    381
    Post Thanks / Like
    Likes (Given)
    121
    Likes (Received)
    210

    Default

    Are you aware the Parker has specs for dovetail O-ring grooves as well?

  13. #12
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,621
    Post Thanks / Like
    Likes (Given)
    1003
    Likes (Received)
    1045

    Default

    Quote Originally Posted by kenton View Post
    Are you aware the Parker has specs for dovetail O-ring grooves as well?
    Harvey's dovetail specs match Parkers, but yes follow Parker's engineering, don't make up your own.

  14. #13
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    151
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    85

    Default

    Quote Originally Posted by markz528 View Post
    This is not exactly a tough sealing application so my other plan is to just machine a rectangular slot that would pinch the o-ring by a few thousandths just so it doesn't slip out. I would determine the depth by trial and error.

    Suggestions?

    Picture of a wooden prototype valve cover adapter and a link to a Harvey cutter.

    http://www.harveytool.com/ToolTechIn...olNumber=23814

    rail.jpg
    I wouldn't do that. The oring has to have room to displace. Look at the % squeeze in the deign guide for static glands. If you need a captive oring, go with the dovetail tool.

  15. Likes doug925 liked this post
  16. #14
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,872
    Post Thanks / Like
    Likes (Given)
    5095
    Likes (Received)
    7677

    Default

    Quote Originally Posted by markz528 View Post
    Thanks! I meant IPM - IPS is a company I deal with........

    The machine is an Atrump bed mill with a Centroid control. My current coolant system is not very good. Bought the machine new around a year ago. Pretty happy with it but there are some things that just need to be a bit better like the cooling system. I bought a good external pump/tank but have not plumbed it yet. I can do that before I do the grooves.
    So - just how much $ did you drop on a brand new POS?
    What could you have gotten good/used for the same price?


    Otherwise - Milland has you covered.
    But in your app, I guess you better stand there with a blow gun and hep it out.


    You may even want to hold the cutter in a holder that you can remove easily.
    If you need to back out once you are in the groove - and started around a corner, getting out will be a nightmare!


    You are expecting to only dovetail one side of the slot, or both?
    I have done them both ways in face groove apps on the lathe.
    I think that I would opt for "one sided" if it was up to me.


    ----------------------

    Think Snow Eh!
    Ox

  17. #15
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    436
    Post Thanks / Like
    Likes (Given)
    29
    Likes (Received)
    235

    Default

    Don't bother with the dovetail style for this application. The Pierson/AB cutter is simple a properly-sized bullnoze endmill with the chamfer geometry already in it. I profile ramp it down and it leaves the perfect channel for a 1/8" oring to press into the channel and seal. I use this for this exact application and it works great. If you're limited on surface area then you may need to get a 1/6" oring cutter instead.

    You don't need to glue the oring into the channel, either, just press it in, trim the ends and glue the ends together, then reinstall by pressing it into the channel and you're good to go.

  18. #16
    Join Date
    May 2010
    Location
    northern Indiana
    Posts
    105
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    itHave done a lot of the undercut o-ring grooves and they work very well. Only problem is that is a pain to change the o-ring then


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •