What's new
What's new

Help with profiling some odd shapes.

gundog

Hot Rolled
Joined
May 31, 2004
Location
Southwest Washington USA
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
 
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.
 
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.
 
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.
 
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.
 
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.
 
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 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
 
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.
 
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
 
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.
 
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
 
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.
 
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.
 
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.
 
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.
 
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
 
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.
 








 
Back
Top