Making a radius punch and die


Page 1 of 3 123 LastLast
Results 1 to 20 of 43

Thread: Making a radius punch and die

  1. #1
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Making a radius punch and die

    I am needing to round the corners of aluminum coil stock up to 0.040" thick but most will be 0.027" or 0.032".Have barely any experience in this area but am thinking of trying to make this myself somewhat as a learning exercise. I may be needing to do up to around 2000 hits but for right now the need is small so I have a little time to try some things. Thinking of doing something like this:

    Attachment 344484

    I need it to be bigger - about 1/2"-3/4" radius. It looks like this is self aligning so it could be used in an arbor press, especially if I extended the lower tube up and put small plates on each side of the opening to control rotation.

    Rather than make the entire punch of hardened material I am thinking of using a piece of hardened material on the end. Perhaps 0.25" thick and pinned to the punch body. One thing I am not clear on is if the projection of the lower die edge into the die is supported below or is self supporting(round hole below). Haven't been able to find a view that shows but my guess is it is supported - which would make the lower body a little harder to make. I couldn't just start with a tube or if I did I would need to add a part inside.

    I am also not clear on how much I need to allow for grinding after hardening and how I would do the grinding. Is it reasonable to do that on a milling machine with a high speed spindle?

    It appears the die edge is pinned to the body or is one of those a screw?

    Any thoughts or suggestions are appreciated.

    Similar Threads:


  2. #2

    Default Re: Making a radius punch and die

    Buy the punch and die and build a press for them I think that would be the way to go



  3. #3
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    For 2000 hits total in aluminum, I would just build a punch & die out of some 4140 or 1050 and wouldn't bother to harden it. That also allows you to change things if you need to. Normal grind allowance after heat treat is 0 to 0.002 or so. Your picture didn't come through so I'm not able to see what you are talking about as far as self aligning.



  4. #4
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Here is another try on the attachment

    Making a radius punch and die-radiuspunch-jpg

    Any other recommendations on material that is a little easier to find in small amounts even if the life will be less? Thinking I may try this in more readily available material and see how difficult it is to make and how well it works. If I could get even a few hundred hits that would be plenty for now. When and if I need the 2000 hits I can make it out of harder material.

    Last edited by Jim27; 12-27-2016 at 08:59 AM.


  5. #5
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    OK, now the picture looks good. It looks like the die is self supporting, and probably the center ''pin'' is a screw, the other two are dowel pins. That looks like a commercially available punch & die. The clue is the tapered notch in the punch. That is a common way of securing a punch into a holder. Take a look through the Dayton Lamina catalogs Punch & Die | Dayton Lamina Corporation Dayton will be happy to make punches & dies, and what you want may be a stock item. A punch & die made from D2 tool steel and heat treated would be good for about 1 million hits before needing sharpening.

    You can buy metals in small quantities from Online Metals at reasonable prices Online Metal Store | Small Quantity Metal Orders | Metal Cutting, Sales & Shipping | Buy Steel, Aluminum, Copper, Brass, Stainless | Metal Product Guides at OnlineMetals.com



  6. #6
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    I ended up getting just the cutting unit here:
    Cornermate

    Their table didn't have the clearance for the parts I needed to cut so I made a couple parts to hold it in a cheap 1/2 ton arbor press. The cutter has the alignment built in so the loose arbor doesn't matter. Works great and was easy on the budget.



  7. #7
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Very cool! Never seen those before.



  8. #8
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Forgot to mention that the cutting edge is shaped so that it doesn't shear it all at once which reduces the pressure needed considerably.



  9. #9
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    1050 or 4140 was previously mentioned. I have another project with similar life needed. I am a bit familiar with 4130 (Dad was into homebuilt airplanes and I had one for a while too, way back when...) but not with other alloys. I found properties for normalized and also for annealed. Think most of this comes normalized if I recall correctly and I think that is the material condition I would want. Is that correct? 4130 looks to be more readily available but also only about 2/3 the hardness in normalized condition.



  10. #10
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Normalized condition would be fine, not that hard to machine. I think you can also get it in a pre-hard condition at around R35C. As I recall, 4130 has a bit less carbon than 4140. I normally used 4140 and 4150 because that's what my local vendor stocked. 4130 should be fine for this application. Later, if it proves to be too soft you can replace the cutting edges with something harder.

    Jim Dawson
    Sandy, Oregon, USA


  11. #11
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    I noticed that some of these materials are typically available in smaller cross sections - i.e. I don't see 1" thick plate available, at least not readily, and I expect it would be costly even for a 10" x 10" chunk. So for a 8" x 8" punch (I have another thread with more detail on that) would you recommend mounting the cutting edges (4130 or whatever) on a block of 1018 or something similar?

    4130 is softer than 4140 but since I don't have a lot of machining experience I think 4130 is a good place to start and I will avoid pre-hard material for now too.



  12. #12
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    If you were to mount the cutting edges on a block of softer steel, the I would use O1 or A2 tool steel as the cutting edges. You can harden thin sections of either with a torch, not the best but a common practice.

    McMaster is not the least cost place to buy from, but you can get small quantities.

    https://www.mcmaster.com/#tool-steel/=1an2j6u

    Another vendor that I use is https://www.onlinemetals.com/

    Jim Dawson
    Sandy, Oregon, USA


  13. #13
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    I see I can get 4130 sheet big enough from a local place in thickness of 0.120", 0.190" and .25". The 0.190 is almost as much as the 0.25 so maybe not as common. Going with a single part would mean I could cut out the entire cutting edge as one part and not have to fit it together in pieces. To be conservative how much overhang can I get by with for the 0.12 material? The other consideration is flex in the flat sheet in the horizontal direction (changes the punch clearance). I can dowel it to the base in multiple places but in considering that I am wondering if I should go with the thicker material? Think I should do the finish cut of the shape after I pin it to the block? I am thinking that would be best for accuracy.



  14. #14
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    So 4130, 4140, etc is available in larger blocks and you were suggesting doing the whole thing as a block with cutting edge of the same piece? I want to avoid grinding if possible.



  15. #15
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    You could use softer material as a base and put the cutting steel on top of it. Two dowel pins would locate it, but use enough bolts to anchor it down. As far as overhang, zero would be best but I would guess the absolute maximum would be about 1/3 the material thickness.

    I would machine the block first, then cutting plate and bolt it to the block. Use standard clearances for the bolt holes to allow a little wiggle room. Then align the punch & die, then drill & ream the dowel pin holes to maintain location. The bolts hold the parts together, the dowel pins do the locating.

    Jim Dawson
    Sandy, Oregon, USA


  16. #16
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Remind me again what machines and tooling you have available. Everything you want to do can be done on a manual mill with a rotary table. But would be much easier on a CNC machine.

    Jim Dawson
    Sandy, Oregon, USA


  17. #17
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    I will be doing this on a Tormach 1100. CNC with spindle speed from 100 to 5140 RPM. Due to radius of curves I will be needing to go down to 1/8" end mill - the ones I have are 2 flute carbide. I also have a ServoProducts mini mill that is very rigid and can run to 20,000 RPM but the travel is only about 4" x 6". Planning to do a small test die on the small on with mild steel before starting on the full size one.

    I confused the issue by posting in this thread but it is really the 8" x 8" odd shaped punch that I am currently working on. Don't think a rotary table is usable for this. I posted here because you had mentioned using non-heat treated steel for punches.

    Since I need a large hole in the base is welding up a base out of square tubing with something like a 1/2" plate on top reasonable? Since I need to get the punched part out after punching I am thinking of blocking this up enough to have about a 1" gap in the front to slide the parts out. That means the front has to be supported from the sides. I calculated a 1" by 1" steel beam will deflect about 0.010 which seems to me to be fine. If I block the other edges up an extra inch I will have it.



  18. #18
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Sounds like you are well tooled to do this so no problem there.

    As long as the 1/2 inch plate is well supported by the square tube, near the cutting edges, it should be OK for light punching. I would like to see pictures of this when it's done. Maybe you could post a build log as you're building it.

    Jim Dawson
    Sandy, Oregon, USA


  19. #19
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    I am thinking I could face the bottom of the tubing to make it nice and flat after welding. But I could also use a 1" plate and just shim it up and not have to weld - I would need to get someone else to do that although I do have a place close by.

    What feeds and speeds would you suggest for 1/8 and 1/4" carbide end mills, depth of cut, etc in 1018 and 4130? The Tormach has coolant but the small one does not. Probably should get larger end mills for hogging out the bigger holes.



  20. #20
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    With the Tormach the best you can get is about for the 1/8 end mill is about 165 FPM, so that translates to about 7 IPM to get a 0.0007 tooth load.

    These are the numbers that I would start out with on my machine, the endmills are so small that the machine HP and mass doesn't really enter into the equation. Then I would adjust after I see how it's cutting. Ramp in where possible. These numbers should be good for both 1018 and 4130 even with the difference in the materials. You're not going for maximum production. Your DOC is really limited by the strength of the endmill.

    1/8 end mill:
    DOC = 0.040
    Step Over 40%
    Cutting Speed ~165 FPM = ~5000 RPM
    Feed Speed ~7 IPM = 0.0007 tooth load

    1/4 End mill:
    DOC = 0.070
    Step Over 40%
    Cutting Speed ~200 FPM = ~3000 RPM
    Feed Speed ~7 IPM = 0.0011 tooth load

    I would also start out with a 3/8 or 1/2 inch cobalt rougher to remove the bulk of the material then switch to the smaller endmills for final profiling. Look at the toolpaths and cut widths. If the small endmills are not going to remove all of the material that the larger endmill left then set the cut width larger than the endmill to do multiple step overs per pass to clean things up. What I mean by this is for the 1/4 end mill you may have to set the cut width at 0.300 or more. If your CAM software has ''Rest'' (as in machine the Rest of it) machining function it should automatically set up the cut widths like I described.

    Jim Dawson
    Sandy, Oregon, USA


Page 1 of 3 123 LastLast

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

Making a radius punch and die

Making a radius punch and die