CNC Fixturing question for 2-sided machining


Results 1 to 11 of 11

Thread: CNC Fixturing question for 2-sided machining

  1. #1
    Member
    Join Date
    Jan 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default CNC Fixturing question for 2-sided machining

    First off, let me state clearly that I am a hobbiest. I am fortunate to have a Series 1 Bridgeport with EZ Vision. I have recently purchased BobCad and took my first 3-day class this week. Having lots of fun making parts in my garage. I'm trying to get some suggestions for machining the attached bracket as I want to mill a fillet on both sides. I've thought about drilling the holes first then milling the outside and top fillet but can't quite get my arms around flipping the part and getting it exactly in the right position to finish the fillet on the other side. Thanks in advance for any ideas.

    Similar Threads:
    Attached Files Attached Files


  2. #2
    Member
    Join Date
    Jul 2005
    Location
    USA
    Posts
    65
    Downloads
    0
    Uploads
    0

    Default Re: CNC Fixturing question for 2-sided machining

    If its a one off and you are making it from plate or bar the right thickness.

    1
    Hold it @ 1/8 deep in vise drill holes a bolt size(3/8 for 3/8-16), pocket through part.
    Profile to @ .01 top of vise jaws then radius/fillet edges.

    2
    Take a scrap plate and drill-tap bolt pattern in it, bolt part down with 1st finished side down.
    Profile down to match finished profile. Radius edges.

    3
    Unbolt part, open holes up to size on drill press.

    If its many parts on 1st side, driil to size.
    For 2nd side, make a set of profiled soft vise jaws to hold finished profile



  3. #3
    Member
    Join Date
    Jan 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by 64dodge View Post
    If its a one off and you are making it from plate or bar the right thickness.

    1
    Hold it @ 1/8 deep in vise drill holes a bolt size(3/8 for 3/8-16), pocket through part.
    Profile to @ .01 top of vise jaws then radius/fillet edges.

    2
    Take a scrap plate and drill-tap bolt pattern in it, bolt part down with 1st finished side down.
    Profile down to match finished profile. Radius edges.

    3
    Unbolt part, open holes up to size on drill press.

    If its many parts on 1st side, driil to size.
    For 2nd side, make a set of profiled soft vise jaws to hold finished profile
    Thanks for the reply. Yes this is a one-off and the material is the correct thickness. I can follow your logic but can’t figure how to set my origin of the part perfectly, since none of the geometry is simple.



  4. #4
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: CNC Fixturing question for 2-sided machining

    Just to clarify, I don't see a fillet on that part, except the radiused corners in the center pockets. But I do see corner rounded edges on both the outside profile and the inside pockets. Is this what you mean by fillet?

    Jim Dawson
    Sandy, Oregon, USA


  5. #5
    Member
    Join Date
    Jan 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: CNC Fixturing question for 2-sided machining

    Yes, that's what I'm referring too. I want to use a corner rounding end mill to add rounded edges in the pockets and outside edges.



  6. #6
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: CNC Fixturing question for 2-sided machining

    I did a part similar to this yesterday. In that case I had two locating pockets and two screw holes to work with. I did the top features in the vise, then did a mirror image fixture for the other side. Because I am eventually going to build 50 parts, I made the fixture out of aluminum. MDF is one of my favorite materials for temporary fixtures. I can take some pictures if you like.

    You have three holes, two pockets, and the outside profile of the part to locate on. Any of those will work. I would bolt a piece of 3/4 MDF to the table and pocket the outside profile about 0.25 deep. Now you have a solid fixture at a known location to work with. You could pre-stage a couple of T-nuts to clamp the part through the center pockets. Clamp from the outside to do the inside profiles and then clamp from the pockets to do the outside work.

    For corner rounding, I normally use carbide tipped corner rounding wood router bits. Take the bearing off and they work great in the mill. I keep a couple of Harbor Freight sets around for that purpose. Another trick I use, and it would work perfect for your particular part, is to use my hand fed router table with a corner rounding bit in the router. Would take about 1 minute to corner round all of the profiles on your part.

    Jim Dawson
    Sandy, Oregon, USA


  7. #7
    Member
    Join Date
    Jan 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Jim Dawson View Post
    I did a part similar to this yesterday. In that case I had two locating pockets and two screw holes to work with. I did the top features in the vise, then did a mirror image fixture for the other side. Because I am eventually going to build 50 parts, I made the fixture out of aluminum. MDF is one of my favorite materials for temporary fixtures. I can take some pictures if you like.

    You have three holes, two pockets, and the outside profile of the part to locate on. Any of those will work. I would bolt a piece of 3/4 MDF to the table and pocket the outside profile about 0.25 deep. Now you have a solid fixture at a known location to work with. You could pre-stage a couple of T-nuts to clamp the part through the center pockets. Clamp from the outside to do the inside profiles and then clamp from the pockets to do the outside work.

    For corner rounding, I normally use carbide tipped corner rounding wood router bits. Take the bearing off and they work great in the mill. I keep a couple of Harbor Freight sets around for that purpose. Another trick I use, and it would work perfect for your particular part, is to use my hand fed router table with a corner rounding bit in the router. Would take about 1 minute to corner round all of the profiles on your part.
    Jim, I like MDF and bit idea. If I make a mirror image into a fixiplaye, how do I make sure it’s positioned perfectly? I can reference and origin off a bolt hole but not sure about the rotation of the part itself.



  8. #8
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: CNC Fixturing question for 2-sided machining

    Quote Originally Posted by RacerJoe View Post
    Jim, I like MDF and bit idea. If I make a mirror image into a fixiplaye, how do I make sure it’s positioned perfectly? I can reference and origin off a bolt hole but not sure about the rotation of the part itself.

    Position doesn't matter. Use your original 0,0 and just cut the pocket. Don't re-zero the machine when you cut the round over. If your machine repeats, then the location will be perfect, it can't miss.

    Jim Dawson
    Sandy, Oregon, USA


  9. #9
    Member
    Join Date
    Jun 2013
    Location
    USA
    Posts
    1041
    Downloads
    0
    Uploads
    0

    Default Re: CNC Fixturing question for 2-sided machining

    I add 2 features to every fixture I want to use more then once. I mill at least 1 edge straight. Then drill or mill and finish a round boss or hole at some known location on the fixture. You can use a locating pin or hole that is part of the fixture already.

    Then to set back up run a indicator down the milled edge and get it perfectly straight. Then indicate the known feature with a test indicator in the spindle and zero your axis. If your known feature is not at part zero then move the axis relative to part zero from your location and zero there.

    Ben

    Sent from my HTC6525LVW using Tapatalk



  10. #10
    Member
    Join Date
    Jan 2016
    Location
    United States
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Jim Dawson View Post
    Position doesn't matter. Use your original 0,0 and just cut the pocket. Don't re-zero the machine when you cut the round over. If your machine repeats, then the location will be perfect, it can't miss.
    Ahhhhhh! Now I think I got it. I was trying to figure out a way to align the part once it’s flipped. It doesn’t matter if I drop the part into the fixture after it’s been machined and run the tool path. So simple, yet I had not thought of it. THANK YOU!



  11. #11
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: CNC Fixturing question for 2-sided machining

    You're Welcome !



    Jim Dawson
    Sandy, Oregon, USA


Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

CNC Fixturing question for 2-sided machining

CNC Fixturing question for 2-sided machining