What's new
What's new

Need suggestions on tooling for a part (10x small tooling)

Fal Grunt

Titanium
Joined
Aug 5, 2010
Location
Medina OH
Have a part I am looking at making for a customer. It's a "fun" job. :willy_nilly:

V

The ID of the part is a V, at the intersection of the V there is a radius, I'll use a #53 drill.

If this were a small production job I would grind a cutter and run the part horizontal, then locate off the V cut to profile the outside.

Cutting the rest of the V is the problem. The part is .618 thick. I would really like to cut it all in one go, flip and take the stock off.

Maybe that is not the most economical choice. This may be a situation where flipping the part and machining it from 2 sides is best?

Going to be making 3-5 pcs.

38B25CD5-0B03-48AF-8F2B-41207D8BEC53.jpg
 
I would go through Harvey Tools and get a small end mill to do the radius unless its a loose fitment and not very critical.
Opt 1 cut the contour about .03 pass the part depth soft jaws and face to size. Sometimes with small thin parts I go to the saw and cut along the contour close without touching the part so the face mill doesnt sling the part out of m jaws.
 
If you can step it down then just get a couple of mills from Harvey, you want a backup in case you break one. Their extended reach stub flute aluminum mills can feed quite aggressively, but be careful about that corner. A couple of HSM passes to clear it out may be in order.

I would take a hard look at milling half depth and flipping to finish. The mills will be a lot more robust in the shorter length. They have a .05" x .4" doc mill that looks good to me.
 
I wouldn't call a .618" thick part a thin part. You don't say what material your cutting. I would go with the cutter or one like David Scott mentioned and flip the part doing the detail in 2 ops.

Standing the part up vertically if that detail is open face and using a form tool would go the quickest, but for only 5.

Just contour it with the little .05" EM in 2 ops, easy.
 
Thanks for the input, sometimes you know the best way, but you just need to hear someone agree.

On a minimum quantity part like this, I really hate to take the time to machine soft jaws. It is so much easier to leave a small base, saw it off, and dust the top with the surface grinder to clean up.

Material is going to be 4340 most likely.
 
Thanks for the input, sometimes you know the best way, but you just need to hear someone agree.

On a minimum quantity part like this, I really hate to take the time to machine soft jaws. It is so much easier to leave a small base, saw it off, and dust the top with the surface grinder to clean up.

Material is going to be 4340 most likely.

If it makes you feel any better, earlier this week I programmed a part that need a .01" endmill and .0115" drill, but only 1/2 hard brass.

I would 'rough' as much as possible with an 1/8 endmill, then pick the corners with something like this -

http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=982160

Then finish, in step downs with a similar tool -

http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=992560

Or alternatively, ( I know you said you wanted to profile and flp) you could 3d surface the V shape with one of these (start with 1/8" or 3/16" maybe) -

http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=17747-C6
 
What's the inside angle? Harvey sells chamfer cutters and runner cutters in all sorts of tight angles. maybe you get lucky and they have a stock size that would work.
 
Have a part I am looking at making for a customer. It's a "fun" job. :willy_nilly:

V

The ID of the part is a V, at the intersection of the V there is a radius, I'll use a #53 drill.

If this were a small production job I would grind a cutter and run the part horizontal, then locate off the V cut to profile the outside.

Cutting the rest of the V is the problem. The part is .618 thick. I would really like to cut it all in one go, flip and take the stock off.

Maybe that is not the most economical choice. This may be a situation where flipping the part and machining it from 2 sides is best?

Going to be making 3-5 pcs.



Maybe I missed something... what does the *outside* profile look like?

PM
 
Hi Fal Grunt:
I'd make this on the wire EDM but if you don't have one and can't get access to one, that's not much help.

But you do have a surface grinder.
So I'd just hog out what you can, dress a wheel and plunge grind the whole shape if you need it accurate and nice.

If you don't particularly need it super nice, you could drill the apex as you suggest, mill it from one side with the smallest convenient cutter, profile the outside in the same op, buck it off to length, surface grind the sawcut end, and then lay it down and pick out the corner with a dressed wheel or even just a hand-ground flycutter

I personally hate profiling with tiny endmills sticking out a long way...you can do it with an extended reach 1/16 cutter but I've usually been better off with a formed wheel, and if you have a good selection of skinny wheels with tapers already dressed on them, modifying one is usually quick and easy, and cheaper than endmills, especially if you can line up all 5 parts in a row and walk through them in one go on the grinder.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Maybe I missed something... what does the *outside* profile look like?

PM

You did not miss anything, I did not describe the outside of the part at all.

Hi Fal Grunt:
I'd make this on the wire EDM but if you don't have one and can't get access to one, that's not much help.

But you do have a surface grinder.
So I'd just hog out what you can, dress a wheel and plunge grind the whole shape if you need it accurate and nice.

If you don't particularly need it super nice, you could drill the apex as you suggest, mill it from one side with the smallest convenient cutter, profile the outside in the same op, buck it off to length, surface grind the sawcut end, and then lay it down and pick out the corner with a dressed wheel or even just a hand-ground flycutter

I personally hate profiling with tiny endmills sticking out a long way...you can do it with an extended reach 1/16 cutter but I've usually been better off with a formed wheel, and if you have a good selection of skinny wheels with tapers already dressed on them, modifying one is usually quick and easy, and cheaper than endmills, especially if you can line up all 5 parts in a row and walk through them in one go on the grinder.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Wow Marcus... That is great advice. I did not even think about using my surface grinder. Just earlier this week I picked up some 3/8" and 1/2" grinding wheels for my grinder. I could rough the part in on my mill and then clean the slot up with the surface grinder. Will have to think about that for a bit!

Wire edm would be ideal for this part, and my preference. Unfortunately I do not have one yet.
 








 
Back
Top