[MetalShavings]

I'm not a complete novice but with some projects I sure feel like one at times.

I have a 770 with all the bells and whistles. I've been trying to find the best way to mill some very small parts
out of 1018 cold rolled flat bar. I've actually already done it with decent success but, every once in while it goes south on me.

It's not the Machine's fault. It's has to do with my skill level or experience.

I'm making some very small parts that are .250" thick. I'm using a 1/4" coated carbide end mill. In order to minimize the post milling work I've used 1/4" metal stock but once my end mill gets to the final layers of my cut, I run the risk of my parts breaking free of the metal stock and either flying off into obscurity in a damaged condition, breaking free just enough to trap and break my small end mill or damaging both the end mill and the parts I'm machining.

I have tried milling these same parts using .375" metal stock and then going back and in the post processing, actually use a metal file to remove the remaining 1/8" of metal to get it down to the 1/4" thickness I need. If I turn my metal stock around and mill off the remaining 1/8" of metal, I run the risk of the same thing happening to ruin my parts. Even though I'm using a larger end mill to plane off the remaining metal, as it reaches the last light passes, the small parts break free to their doom.

Please don't ask me to post my CAD or CAM files. I really don't want to do that at this time. I will post a pic of some of my prototype parts in order to give you an idea what I'm trying to describe. What I'm really asking is, how would you more experienced guys go about setting up your cutting paths for such small thin parts?

Picture trying to machine eight 3/4" x 1/4" thick trianglular parts from a piece of 1/4" thick by 1 1/4" wide metal stock. The actual geometry is a little more complex than a triangle. I'm just trying to paint a mental image for you.

Tim M.

[SCzEngrgGroup]

Use a bar of thicker material - 3/8" should do - held in a vise by about 0.100". Mill all your features. Then cut them apart with a bandsaw, turn them upside down, hold in soft-jaws milled to match the part profile, and mill off the extra 1/8".

Regards,
Ray L.

[Steve Seebold]

I'm pretty good with small parts and small cutters but if we can't see what you're doing, it's impossible to give you any ideas.

Good luck.

[SCzEngrgGroup]

I'm pretty good with small parts and small cutters but if we can't see what you're doing, it's impossible to give you any ideas.

Good luck.

You could try looking at the photos he posted....

Regards,
Ray L.

[Steve Seebold]

I hadn't seen his pictures, but aluminum soft jaws machined to fit should work just fine.

[phoneman]

Clamp a piece of alu tooling plate down to your mill table. drill and tap blind holes in all the locations we see counter sunk hole in the photo. clamp your work piece to the tooling plate. Drill and counter sink the holes then install counter sunk screws in holes and do profile to depth. screws will keep parts from flying out of machine and causing any of the problems you talked about.
I do this all the time.

[SCzEngrgGroup]

Clamp a piece of alu tooling plate down to your mill table. drill and tap blind holes in all the locations we see counter sunk hole in the photo. clamp your work piece to the tooling plate. Drill and counter sink the holes then install counter sunk screws in holes and do profile to depth. screws will keep parts from flying out of machine and causing any of the problems you talked about.
I do this all the time.

Those screw holes are in the waste material between the parts. There are no holes in the parts....

Regards,
Ray L.

[phoneman]

Ray
You are correct the counter sunk holes are in the waste. Do I not also see holes in the parts that are not counter sunk that could be used.

Dave

[SCzEngrgGroup]

Ray
You are correct the counter sunk holes are in the waste. Do I not also see holes in the parts that are not counter sunk that could be used.

Dave

Yes, you're right. But holding steel parts for milling with a single small screw is not going to work well... And when one let's go, it'll surely break the tool every time.

Regards,
Ray L.

[pickled]

Flip and machine off the carrier while holding the stick of parts in soft jaws.

[phoneman]

Ray
That is true if your DOC for the final cut is more than the screws can handle. If you make that last pass very thin then I don't think you will run into trouble. This would be faster than doing a second op in soft jaws.

Dave

[AUSTINMACHINING]

Using .375 stock, face, mill to full, depth + .01 leaving .007 on the wall for a finish pass .Finish and break edge .005. Flip part in soft jaws machine away carrier and break edge.

To make my soft jaws, after machining holes, I camp together and face both jaws in one pass. Then mill mirror image +.001 of part profIle array.

[Philbobb]

Tabs would work. I don't know what CAM you use, but if it's Fusion 360 or one of the HSM versions tabs are easy to do in CAM. Machine the top side, break the parts free of the tabs and file the tab remnants, or flip them into soft jaws and machine. Or you could flip them onto a fixture plate that holds with a screw through the hole, and uses a couple short pins to keep the part from rotating. The big advantage with this is you could potentially finish more parts in a setup then flipping the whole bar into soft jaws.

[Steve Seebold]

Yes, you're right. But holding steel parts for milling with a single small screw is not going to work well... And when one let's go, it'll surely break the tool every time.

Regards,
Ray L.

Hey Ray, why not make a simple fixture using MiteeBites for clamping.

I use them a LOT and they make for some really quick and dirty tooling that you can toss when your job is finished or save it in case the job comes along again.

[SCzEngrgGroup]

Hey Ray, why not make a simple fixture using MiteeBites for clamping.

I use them a LOT and they make for some really quick and dirty tooling that you can toss when your job is finished or save it in case the job comes along again.

That would certainly work if he's making enough of them to justify the time and expense of making the fixture. Mitee-Bites are great - I make my own frequently.

Regards,
Ray L.

[keen]

Can you make them back to back on thicker stock - If you have to make many.

See Video at 1.43 in. Keen

https://www.youtube.com/watch?v=4roh8UHRwIk

[daniellyall]

make up a set of soft jaws it be safer. drill hole profile 2/3 flip, finish last 1/3 in soft jaws

[mountaindew]

Raw material thickness can vary in my experience. In order to get accurate part dimensions the method ray or Austinmachining details would work well for both the holding problem and could provide you with a more accurate 2 sided finished part with a correct or controlled thickness or z depth. I would also consider cutting the raw stock into smaller pieces or employ some strategy to avoid milling so many slots. Might require user to load more raw stock into vise but shorter machine cycles "less tool paths" could speed up the production overall. If hundereds are required then custom fixture plate and big sets of softjaws would be on top of list.
something to consider

[BAMCNC.COM]

Softjaws, I have at least 40 videos on Soft Jaws alone if you need ideas.

[MetalShavings]

Maybe I should have worded my original posts a little differently. I thought I had mentioned that I tried thicker metal stock and flipping the part to plane off the remaining stock. I think I've tried nearly everything that's been suggested thus far except for the "Tabs" idea and the "Soft-Jaws" idea. I even tried holding my metal stock with counter sunk screws as well; as evidenced by one of the pics I uploaded.

I'll be redrawing my final version of these little parts soon. I'll give the tabs idea a shot before trying to make up some soft-jaws. The parts in question only get made up once every couple of months or so. It's not mass production by any means. I was just hoping to either eliminate or at least mitigate the post machining process I've been having to do on these little parts. Grinding off some tabs may be less work than filing down the back side of my metal stock. Ideally, I'd like the Tabs to keep my parts from breaking loose and being damaged as well.

Even when I do have to spend time hand filing them to the proper thickness, I can still get a batch done in less than one day. It would be nice to be able to mill them once and be done with them though.

I was really hoping that there was one of those easy but elusive remedies to this situation that some of you old machining sages could drop on me. I guess there's no easy fix this time.

Many thanks to everyone who took the time to post. I appreciate it.

MetalShavings