Making a radius punch and die - Page 2


Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 43

Thread: Making a radius punch and die

  1. #21
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Very helpful! I know there are speed and feed calculators all over but it seems everyone has some adjustments to this for material, cutter, and various reasons. Your numbers seem conservative to me and that's perfect - as you say this isn't production.

    The small mill is very rigid but limited in torque - it uses a rubber oring belt - similar to used on Sherline products I think. For that reason I plan to reduce the DOC - I am thinking to about 1/3 of what you gave. Long term I may replace the spindle with a trim router if the belt drive is too limiting.

    Any advice on lube or coolant? Really just an issue on the small machine. I could use air on the small mill to blow chips away to minimize recutting chips. Is dry cutting ok?

    The local supply has A36 in 1" thick plate. They may have 1018 but it's not on their site. I see A36 is somewhat weaker than 1018 but for this I am thinking it will be ok since I am not approaching yield strength - yield is considerably lower.



  2. #22
    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 coolant, I use kerosene for most everything. It's what I have in the tank because I do a lot of aluminum. I have a fogless spray mist type coolant system that I built. I normally apply the coolant at about 1/2 cup per hour. At that application rate, it just evaporates so no mess. I don't like the water based coolants for the work I do. Cutting oil from the local hardware store works also, will work in some spray mist systems if thinned with kerosene. For really light work and engraving I use soy oil (cooking oil) applied with a brush or oil can. Apply enough air to blow out the chips so they are not being recut and jamming up the end mill.

    I use a lot of A36 just because I have a lot of it kicking around. I'm sure it will work fine in place of the 1018.

    Jim Dawson
    Sandy, Oregon, USA


  3. #23
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    I would be interested in your mist system. Do you have a build log online?

    The large mill isn't mine. Part of a local workshop I am a member of (was TechShop before it recently folded and the local one is now independent. The others are to be reopened with a new owner). So I have to use the coolant they supply. Some sort of water based stuff I think. Also why I can't grind on it.

    For the small mill I will use cutting oil or soy oil in an oil can. I need to mount some flexible nozzles for mist and lube but for now I can rig something up.

    I will try to do a build log for this die - good suggestion.

    Related to the feeds and speeds... climb or conventional milling?

    One thing I haven't quite worked out is how to hold the sheets for milling. Because of the size I will only be able to clamp on the ends with simple T slot clamps. I plan to shim the material off the table with some 1/2" material scraps. The 1" plate will be plenty rigid but the 0.120 sheet needs more support. I could use some bars along the sides and sandwich it between two bars. I suppose the bars could even be hardwood? Wood is a lot easier for me to work with than metal and cheaper too. There are probably better ways to do this. Any suggestions? I considered adding some holes where it doesn't matter for additional hold downs. for accuracy I want to do all the outline and dowel holes without having to remount the part on the table.



  4. #24
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Here is a link to the meat of the design Digital Mist Coolant Pump | The Hobby-Machinist Forums You might read through the whole thread. The system will run with or without the pump. You can adjust the flow with a flow control rather than a pump, I'm just using the pump so I can control the flow from a slider on the screen.

    Grinding on a mill is not the best for the mill because of the grit. Requires that the grit be captured and controlled, not easy to do. Mechanically the mill would do the job.

    As far as hold down and spoil board under the sheet. That's easy. I use 3/4 inch MDF for the spoil board, it handles oil based coolant well, never tried it with water based coolants. First clamp the edges down as you planned, then drill all of the holes first. Then use the holes to screw the plate down to the spoil board. I use drywall or deck screws, or in some cases wood screws to hold parts to the MDF. Whatever works for the application. I normally screw the spoil board down to the table using flat head cap screws into the T-nuts and countersink the screws well below the surface.

    Here is a picture of some 0.125 thick 316 SS parts I did on a MDF spoil board. I used 5 screws per part because there were 5 holes in the design, but 2 screws would have held them just fine. BTW, for this job I used a 3/16 straight flute router bit, worked fine and is still sharp. These were roughed out with a hole saw then profiled. I drilled all of the holes first, then screwed the parts down, then did the other machining.





    Attached Thumbnails Attached Thumbnails Making a radius punch and die-img_0718-jpg   Making a radius punch and die-img_0713-jpg  
    Jim Dawson
    Sandy, Oregon, USA


  5. #25
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Looks good. They don't want wood cut on the mill so I am not sure what they are going to think of this but it seems like a good idea to me. Seems like the mdf would swell with the coolant so maybe just a board or scrap of plywood?



  6. #26
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    I have used aluminum plates under also or an aluminum plate supported on square bars. Just drill & tap rather than using wood screws. Sounds like you need your own mill. Wood can be a bit messy on a mill.

    Jim Dawson
    Sandy, Oregon, USA


  7. #27
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    My own mill would be great but I'm not sure where I would put it. Hopefully someday. To avoid having to tap the holes I need to get some self taping screws.



  8. #28
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    It took me a lot of years to have enough room for shop space. I just set that as my end goal. Now I have 1200 sqft (30x40) and it's still not enough. I keep buying more machines.

    If you are going into a aluminum or steel plate, thread forming screws are what you want if you don't want to tap. https://www.mcmaster.com/#thread-for...crews/=1ao5sty

    For sheet metal I use self-drilling screws a lot. https://www.mcmaster.com/#self-drilling-screws/=1ao5tuh

    BTW, this is how I control the dust when working wood on the mill.



    Attached Thumbnails Attached Thumbnails Making a radius punch and die-img_0261-jpg  
    Jim Dawson
    Sandy, Oregon, USA


  9. #29
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    That should keep the dust down!

    I was planning to use 1/8" plate for the cutting edges but need to recess the hold down heads and that doesn't give enough thickness for a counterbored hole for a allen head cap screw with either a button head or a short head - either one in a 10-32 takes about 0.10" for height. Looks like my choices are 1/4" plate or flat head screws. Flat head screws concern me as they require more precise location - the other types give a small amount of movement. But I suppose if I am locating them with CNC at the same time as everything else that won't be an issue.

    If I do the hole and tapered part for the flat head with a center drill I was a bit concerned with getting the height right but some measuring of the tool should take care of that. Or I could just mark the center with CNC and do it by hand later. If I use the CNC what plunge rate for the center drill?



  10. #30
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Was just reading up on center drills vs. spotting drills and that spotting drills are the best for this. I will be getting spotting drills for this so the question becomes what is appropriate speed and feed for drills in various steels. I am guessing those numbers for spotting drills are the same as for standard drills.



  11. #31
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Flat head screws almost eliminate the need for dowel pins because they locate the part as well as hold it together. Precise screw hole location is not as critical in this case because you are going to do the final profile after the plate is mounted to the base. With a CNC you will be able to have exactly the same hole pattern in both the base and the plate. In fact, I would clamp the two together and drill the screw holes in both in the same setup. Can't miss that way.

    Spotting drills are really the correct tool to use for starting holes, but I use center drills because that's what I have. You are not going to to do the countersink with the spotting drill, English flat head screws are 82° and metric are 90°. So you are going to need a countersink, my favorites are single flute or 0 flute from M.A. Ford.

    https://www.mcmaster.com/#countersinks/=1ap1fhk

    https://www.mcmaster.com/#countersinks/=1ap1frg

    In this case, because your plate is only 0.125 thick, you only need to drill at the tap size because the countersink is going to go all the way through the plate and slightly into the base because of the head height of the screw. This is perfectly acceptable and works well, assures positive locating. The head height on a 10-24 is 0.127, and on a 1/4-20 is 0.161 unless you are using undercut screws. So for a 10-24 you are going to want to go about 0.140 deep.

    You can calculate the depth or just eyeball it. Turn countersinks slow, like a reamer, use cutting oil. For the spotting drills use normal feeds and speeds.

    Jim Dawson
    Sandy, Oregon, USA


  12. #32
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Good points on locating.

    Spotting drills are available in 82 degree but not as common as 90 or 120 (at least from what I can see) so I could go that route or a countersink. But the 82 degree spot drill doesn't work well for spotting locations to drill unless I go in past the point. That doesn't seem practical since a lot of the holes I need to drill are smaller than the size I need to countersink. I can also get spotting drills in 120 degree which (apparently) is needed so the angle is larger than the drill tips and they truly center in the depression. In any case, I need two tools, one to countersink and one to mark start locations. Seems like a 82 degree spotting drill would be easier/quicker for countersinking - I could drill the holes I need countersinking on to the needed depth and for hole locations that need drilling only go in enough to form a guide dimple.



  13. #33
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Either way would work fine. It's the end result that counts, it doesn't really matter how you get there. I would do whatever is the most efficient way for a particular job.

    Jim Dawson
    Sandy, Oregon, USA


  14. #34
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Did a small test with my desktop mill with a 1/4 end mill and mild steel - success! . Feed per tooth 0.0008 and DOC 0.020. Speed 3000. It didn't stall but did sound like it was bogging down at a couple of points so I will lighten up the DOC a bit. To get speeds above 4000 I need to change the belt location and won't have as much torque so may just leave it at 4000 for 1/8" cutters. If I was going smaller (which I will be doing at some point) I will change for high speed. Used some air for blowing the chips away - think I will get some flexible hose and fasten it to the head so I don't have to hold the air the whole time. For the full size parts and the 4130 I will be using the Tormach so I can take bigger cuts.



  15. #35
    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 have it under control. You could run the 1/8 inch at 4000, just cut the feed rate back to match to keep the tooth load in a reasonable range.

    Jim Dawson
    Sandy, Oregon, USA


  16. #36
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Got some steel from a local place. 4130 for edge is marked "4130 HARD". It was sheared to size so it must not be fully hardened. Is this what is called prehard? I am going to try some test machining on it. I need to cut it to rough size - any issue with bandsawing this? I also need to bandsaw the base plates. Found a deal on a cutoff that is rusty. I wire brushed off what I could and will sandblast it but its a bit large to get in the blast cabinet so I planned to bandsaw it first. The rust will be a bit hard on the saw blade but I don't think too bad. I could mill off the rust but think blasting it first would be less wear on the cutters.



  17. #37
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    It could be prehard, a file test might tell something. I have found that it's possible to cut almost anything with the right cutters. I have band sawed some pretty hard stuff using bi-metal blades. The rust should not be an issue for milling unless it's pretty deep. Mill scale is like carbide and you have to get under it on the first pass to keep from dulling cutters. Sand blasting is a good idea.

    Jim Dawson
    Sandy, Oregon, USA


  18. #38
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Well, I cut up the 4130 with no problem on a bandsaw. The 1" plate was a different story. I started in but only got a bit in and stopped for fear of completely trashing the blade and even if not that then taking forever. Don't have access to a torch (although maybe can find someone...) Considered putting it on a Bridgeport (at a maker space) and milling through it. I can file the edges without much trouble so not hardened but think it is harder than 1018 (very rough hardness guess). Any suggestions?

    Used to have access to a horizontal bandsaw but no longer. If I could get it clamped in vertical and cut from both side I think that would work. Nice thing about that is it feeds automatically. Cut some fairly hard 2" shafting nicely but from the speed of that I would be about 15 minutes for a 12" cut in this plate.

    My guess is a plasma torch would be ideal but don't have access to one. But I think I could find one.



  19. #39
    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 don't want to cut that with any kind of heat. The edge will harden and you'll be doing a bunch of grinding before you can machine it. I'm sure it's much harder and tougher than the 1018. Any kind of a band saw would work, as long as it will physically fit. Cutting it on the BP would work also, I would use a 3/8 cobalt rougher end mill for that. You could cut 1/2 inch deep at the full 3/8 width.

    Jim Dawson
    Sandy, Oregon, USA


  20. #40
    Member
    Join Date
    Aug 2012
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Default Re: Making a radius punch and die

    Two edges were cut with some sort of torch. I can grind off a bit to get through the harder part although it doesn't seen much harder. How deep should I grind to get through the hardness?

    I got a 1/2" cobalt rougher (actually 2 in case I break one...). Next issue I see is how to mount this to cut clear through. It is bigger than the table is wide so I can only clamp at the ends without some fixture. I am thinking I could space it off the table with some scraps of 1/2" aluminum or something similar. Then mill a slot half way across the plate. I could then put a clamp or clamps in that slot and mill the rest of the way. If I put the T slot nuts in place before starting I might even be able to add the clamps without loosing my location.

    I am thinking I want to make the cuts in the X direction so I can use the power feed to get even feed. If I do that perhaps I could center the cut over the table and use the outside T slots to clamp and not have to change anything while cutting. But there will be a fair amount of metal hanging off the table. I am thinking I should still mill part way and put a clamp in the center slot to help support things but maybe I am being overly cautious.

    Planning to do this manual lube/coolant. The mill doesn't have coolant system but I can give it a shot occasionally.

    I am not really concerned about edge finish. How rough is the finish going to be? I could clean it up with a standard mill but will skip that unless it is really rough.



Page 2 of 3 FirstFirst 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