Help with profiling some odd shapes.
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 30
  1. #1
    Join Date
    May 2004
    Location
    Ridgefield, Wa USA
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    187
    Likes (Received)
    69

    Default Help with profiling some odd shapes.

    I have some new parts I am prototyping for my business and they are odd shaped parts, the parts will be cut from .375" 6061 I have read about profiling but not cutting all the way through then flipping the blank to the opposite side and surface cutting the blank until the part drops out. I have never tried this the parts are roughly 5" x 3" overall but in an irregular shape. How deep would you usually cut the profile before flipping the blank to surface cut the other side? I will attach a picture of one of the parts.

    front-profile.jpg

  2. #2
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,527
    Post Thanks / Like
    Likes (Given)
    979
    Likes (Received)
    1014

    Default

    How many of each are you doing? How important is the surface finish of the sides where the end mill cuts come together? Several ways to skin this cat, which way works best depends on some details. That does look like fun. A double station vise, like a Chick, would be perfect for holding this one.

  3. Likes gundog liked this post
  4. #3
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,185
    Post Thanks / Like
    Likes (Given)
    379
    Likes (Received)
    539

    Default

    Agreed many ways to approach this. Quantity would be the biggest determining factor. if its just a few pieces then OP 1 would be .5 material, face profile .385 deep then OP 2 would be double side tape or super blue to flat surface and just of back side then hand deburr.

    If there are several then a soft jaw for OP 2 that way you can chamfer the backside as well. A two station vise would be great, but two regular 6" vices will work just fine.

  5. Likes gundog liked this post
  6. #4
    Join Date
    May 2004
    Location
    Ridgefield, Wa USA
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    187
    Likes (Received)
    69

    Default

    I plan to make batches of about 50 in one run, when I get the design finished and working the way I want them too. I planned to add some holes to bolt them to a sub plate but I would really rather they did not have the holes in them. I could also leave some tabs and trim them out but I was curious about the method I asked about I have never tried that.

    I would like the parts to have a nice edge finish or I would have them water jet cut there is also one other part that is odd shaped and it has tapped holes in it. I made one of those today and used a sub plate to hold it using the tapped holes in a second op for the profile cut.

  7. #5
    Join Date
    Jan 2003
    Location
    Posts
    272
    Post Thanks / Like
    Likes (Given)
    22
    Likes (Received)
    64

    Default

    Best bet would be 0.5" stock and soft jaws for OP2 as others suggested.

    Another quick and dirty trick I like to use sometimes is to use same size stock (0.375) and machine the outside to a depth of say 0.340 and leave a few thou on the walls. Then do one more pass right to size, and all the way through, but stop short of endpoint leaving a single thin tab holding the part which can be filed/sanded after. Put your start/stop point against fixed jaw so part doesn't move much when its mostly cut out.

  8. Likes gundog liked this post
  9. #6
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,185
    Post Thanks / Like
    Likes (Given)
    379
    Likes (Received)
    539

    Default

    50 pieces just make some aluminum jaws for the second OP then cut out out 2 female images and get two off in one shot.

    I would like the parts to have a nice edge finish or I would have them water jet cut
    If it is just edge profile that you want to look nice then blow them out nested then chamfer the profile in aluminum jaws. You would save a load of time and material that way.

  10. Likes gundog liked this post
  11. #7
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,692
    Post Thanks / Like
    Likes (Given)
    304
    Likes (Received)
    1807

    Default

    I hate shit like these!

    Not because the part is difficult to make, rather 'cos the engineer/buyer assumes that a 3/8 flat stock is all it's needed to make one, few, few tens or millions of them!

    Here, I'd start with a 1/2" stock, make complete on all then flip and face to length. Regardless of qty!

  12. Likes thomj, 360427, gundog, mhajicek, 52pickup liked this post
  13. #8
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,185
    Post Thanks / Like
    Likes (Given)
    379
    Likes (Received)
    539

    Default

    I dug up a video of some parts we do in batches of 100 a week. It worked out cheaper to have them blown out of plate nested rather than bar stock. Then just soft jaw and be done with it.

    YouTube

  14. Likes gundog liked this post
  15. #9
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    468
    Post Thanks / Like
    Likes (Given)
    31
    Likes (Received)
    163

    Default

    Quote Originally Posted by SeymourDumore View Post
    I hate shit like these!

    Not because the part is difficult to make, rather 'cos the engineer/buyer assumes that a 3/8 flat stock is all it's needed to make one, few, few tens or millions of them!

    Here, I'd start with a 1/2" stock, make complete on all then flip and face to length. Regardless of qty!
    I used to agree with that 100% until the last few years. My customer supplies flat plate stock(not bar stock),it took me a while of quietly cussing to my self, but once I came to the sense of not using vises for everything it all clicked.
    its alot faster you get no bow in the part, and you dont have to worry about crappy finishes. all it takes is a fixture plate and a clamp here or there. most cases you dont have to flip over the part.
    then the next time you need to make some you just put your fixture plate in the vise and your ready to go.
    most of our jobs take less than 30 mins to set up anymore, unless Its the 1st time we do it and have no fixtures.

    this job is a perfect candidate for plate stock and 2 made clamps and some 1/4-20 or 10-32 screws and a batt operated driver.

    plate stock is completely different than BAR stock for some who dont know.
    dont get me wrong I still use vices but mainly vacumm plates and fixture plates we do tons of plate work.

  16. Likes primeholy, DavidScott, gundog liked this post
  17. #10
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    2,619
    Post Thanks / Like
    Likes (Given)
    191
    Likes (Received)
    1922

    Default

    I never fell into the thicker stock routine, additional stock cost, time and fixturing.

    If this were a part for me you could bet there would be two holes in it to mount the blank to a fixture plate[which is just an end cut of this very stock held in a vise]

    CAD CAM allows tabs machining, which is pretty easy and fast. tabs can be cleaned up with a file, or if it needs to be fussier, I would probably CNC back bur the part in soft jaws

  18. Likes gundog liked this post
  19. #11
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    7

    Default

    With there being no holes in the part, I would lean towards thicker bar stock, use two vises, one to face and profile, next with machined soft jaws to deck to thickness, and chamfer if needed. Looks like you will have to be mindful of how you clamp in the second op, so you don't deform the part.

  20. Likes gundog liked this post
  21. #12
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,074
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    1424

    Default

    P1 with Talon Grips grabbing 1/2" stock, then you can run fast and hard
    P2 soft jaws (maybe with an acetal insert slipped between the forks to keep them from collapsing)

    You get a fully machined part, fully deburred in the machine, no blend lines, no worries about scratches on the stock or the stock coming in bowed, cupped, or off-size.

    Regards.

    Mike

  22. Likes gundog liked this post
  23. #13
    Join Date
    May 2004
    Location
    Ridgefield, Wa USA
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    187
    Likes (Received)
    69

    Default

    Quote Originally Posted by SeymourDumore View Post
    I hate shit like these!

    Not because the part is difficult to make, rather 'cos the engineer/buyer assumes that a 3/8 flat stock is all it's needed to make one, few, few tens or millions of them!

    Here, I'd start with a 1/2" stock, make complete on all then flip and face to length. Regardless of qty!
    These parts are designed by yours truly the parts are for a new product. The thickness is not that critical 1/4" would probably work your method is what I was trying to describe. I am a self taught guy and fixturing is something I struggle with but I am learning.

    I can't get my head around using soft jaws to do the outside profile. I use soft jaws in my vises and can make some for this part if needed. I usually make pretty simple parts and I have dedicated fixture plates that use holes in the part to hold the part for second op profile cutting but this part has no holes and I don't really want to add holes to fixture them.

  24. #14
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    7

    Default

    Quote Originally Posted by gundog View Post
    These parts are designed by yours truly the parts are for a new product. The thickness is not that critical 1/4" would probably work your method is what I was trying to describe. I am a self taught guy and fixturing is something I struggle with but I am learning.

    I can't get my head around using soft jaws to do the outside profile. I use soft jaws in my vises and can make some for this part if needed. I usually make pretty simple parts and I have dedicated fixture plates that use holes in the part to hold the part for second op profile cutting but this part has no holes and I don't really want to add holes to fixture them.
    With the soft jaws, you cut the outside profile of the part into the jaws so you can hold them firm, and repeat. You may have to go with bigger soft jaws,depending on how you want to hold the part.If you are using traditional kurt style vises, put something in between the jaws, can be whatever thickness necessary. I use anything from 1/8 inch parallels up to 123 blocks. Lay it out in your cam software with your jaws modeled up also and move the part around till it seems it will hold well. You can modify the shape you cut, just think about chatter, like having enough contact points.

  25. Likes gundog liked this post
  26. #15
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    7

    Default

    YouTube
    Here is an example I found quickly to give you reference. Your part is going to be a little more tricky to hole, but I think you can figure something out.

  27. Likes gundog liked this post
  28. #16
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    7

    Default

    Also, if it is a job you are going to be tearing down and setting up, you could put two 1/4 inch dowel holes in your jaws when you make them initially, and install them with the (long)dowels going in each jaw to locate, and modify your allen wrench so it will fit between the two.

  29. Likes gundog liked this post
  30. #17
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    7

    Default

    YouTube
    Here's another

  31. Likes gundog liked this post
  32. #18
    Join Date
    May 2004
    Location
    Ridgefield, Wa USA
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    187
    Likes (Received)
    69

    Default

    Quote Originally Posted by primeholy View Post
    YouTube
    Here's another
    Thanks that does help I have a new way to think about the soft jaws.

  33. #19
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,527
    Post Thanks / Like
    Likes (Given)
    979
    Likes (Received)
    1014

    Default

    I think the way I would make these parts is to cut the inside of the U section only then clamp it to a plate that registers the U section for location and to help hold it tight. The fixture island to register the part only needs to be .1" tall or so. The clamp should be the U section with a flange to contact the top of the part. Not because the clamp needs to register to the part but to give the clamp more strength without it sticking above the part more. The clamp flange should be .187"-.25" thick, or so. Hold the clamp in place with 2 ea 1/4-28 bolts. I would do this to prototype the parts because part of prototyping the parts is to prototype how you are going to make them efficiently. This is still 2 ops but you can either use bar or bigger plate to make them. With bigger plate you could play around with nesting the parts together with the U sections intersecting perhaps, you only need .2" between any part surfaces for a 3/16" mill. I would use a corn cob rougher to rough the parts out in 1 or 2 passes to full depth with said 3/16" x .375" loc mill. If using bar then I would use a 1/4" corn cob mill to rough.

    I am assuming you don't need to face the parts and I am assuming you can tumble them to deburr. I think this would be the cheapest way to make these parts while maintaining cosmetically excellent machined surfaces and you could hold around .001" tolerance if needed.

    To drive any screws the tools in the photo are the way to go. They take 1/4" hex bits, are torque controlled, shut off once the screw is torqued down, and run around 800-2000 rpm so they are pretty fast. New they are around $1200-$1500, used on Ebay $40-$90. If you have these and battery drivers the battery drivers will sit on the shelf collecting dust. These are easily one of if not the best value investment I have ever made in my shop. All of mine are Uryu because I think they have the best feel, are extremely well made, parts and service are available, all of the manuals or any other literature is easily downloaded off their website, and the US headquarters is about 70 miles away.

    a3.jpg

  34. #20
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    2,619
    Post Thanks / Like
    Likes (Given)
    191
    Likes (Received)
    1922

    Default

    DAmn if they are your parts, drill two tooling holes

    Look at the time difference, drill two holes 5 seconds, flip to second vise to turn the part to chips

    mill from thicker stock, 33 percent more stock cost, time to face the whole thing down, fixture time


    I will have a dozen of these made before you finish the fixture.


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
  •