Help Forming an Odd Internal Profile

I have a project which requires making two bushings out of acetal plastic that have an odd internal profile cut into them. My first thought was to make a broach from 4140 prehard and jam it through, but the resulting hole was sloppy and the profile changed size through the process. The middle diameter is smaller at the end than the beginning, pushing the mating part against the larger diameter and leaving a gap on the flat, before completely jamming up halfway through the bushing. One of the shoulders is also poorly formed, not in line with the other side and the center.

The profile is a flat .100 from center meeting a diameter .250, and a semi-circle of .285 cut out of the half opposite the flat. Pilot hole is .200 with the flat cut tangent on the broach. Profile length is .750, but it is technically blind so I made it the full .850 and plan to press fit a slug into the back to make the shoulder.

I'm wondering if I might get a better result trying to make two separate broaches, one to make the .250 diameter with the flat on the bottom, and then using that as a pilot shape on a completely separate broach to carve out the semi-circle.

Here's a picture of my first attempt, and a screenshot of the part I want (pressed slug will be going in from the side shown). Ideally, I want to get ±0.002 on the diameters, but my first attempt is pretty discouraging for that accuracy. Semi-circle shoulders can float a bit (maybe ±.010), but having accurate diameters is pretty important.

Any suggestions on making multiple parts and fitting them together should come with the caveat that it needs to be fluid tight from inside to outside.

Email a drawing to [email protected]. He'll make you a broach that will do exactly what you want to the tolerances you want. Some peck broaching, and you're good to go.

TeachMePlease said:

Email a drawing to [email protected]. He'll make you a broach that will do exactly what you want to the tolerances you want. Some peck broaching, and you're good to go.

Click to expand...

I have no doubts of that. Unfortunately, I don't think the budget for this project can support a custom-engineered tool from an outside source for just a couple pieces. I was planning to use the down time from the current slowdown to make it happen. I am prepared to do some hand-fitting, but my first attempt was a bit too far off the mark.

Can you make a steel rod of the correct but slightly oversize male form, and press the acetal plastic into conformance while hot, pushing or pulling the steel form out whenever it's easy enough?

Might try making a slip-fit steel sleeve to support the part for broaching. I think that thing is not rigid enough to broach without moving around.

Turn the OD, put in the pilot hole, then drop it into the sleeve to broach?

Joe Gwinn said:

Can you make a steel rod of the correct but slightly oversize male form, and press the acetal plastic into conformance while hot, pushing or pulling the steel form out whenever it's easy enough?

Click to expand...

Interesting idea. Might even be able to do the blind profile properly that way. I just wonder how much internal stresses are going to move things around when I go to finish the diameter, as it isn't very thick.

guest said:

Might try making a slip-fit steel sleeve to support the part for broaching. I think that thing is not rigid enough to broach without moving around.

Turn the OD, put in the pilot hole, then drop it into the sleeve to broach?

Click to expand...

I used .500" diameter at the time of broaching planning to finish OD afterwards for that reason, but you might be right, it's probably not enough. I could either try using 1" stock, or the sleeve, maybe with smaller teeth. I currently go from .200 to .285 in 9 steps on half the part, and the opposite side remains nearly untouched. Maybe I just need to stiffen it up and take smaller bites after all.

Edit: I did basically use that method, but only 1/8" deep on the bottom. The top was unsupported. Since it is a non-symmetrical shape, I bet there is some movement somewhere.

Bore hole to fit OD in a block to drop part into for broaching. I bet that part is swelling as you are pushing on it. Add more positive rake to the broach and hone that sucker razor sharp. If that still tears out, the broach is far too aggressive and might be a good idea to make a second broach for finishing, one longer broach/more teeth would work too.

Rotab & milling machine

1, Bore largest hole you can without fouling any feature.
2 Make up a plunge/push cutting tool from (say) 3/8 drill rod, ..the end looks a bit like a hex wobble broach but with out the hex.
3 Mount blank in chuck of rotab and do as much as you can with the round push tool, just use the quill down feed.
4 Make up smaller tools to cut the angle and sharp corner details.

NB, By keep the cutting edges of tools of a known diameter, surprisingly high accuracy can be achieved straight off the dial

I once (well, actually twice) had to make a similar size 13 spline metric sleeve. I machined close to tolerance, and then, Horrors!- I filed it. Test fit with male part, file a bit more, until done.
Old school- like they make German Apprentices do before they let them touch any electric tools.

Works fine, just takes time and patience, and, a drawer full of files going down to jewelers files.
All of which I had.

Limy Sami said:

Rotab & milling machine

1, Bore largest hole you can without fouling any feature.
2 Make up a plunge/push cutting tool from (say) 3/8 drill rod, ..the end looks a bit like a hex wobble broach but with out the hex.
3 Mount blank in chuck of rotab and do as much as you can with the round push tool, just use the quill down feed.
4 Make up smaller tools to cut the angle and sharp corner details.

NB, By keep the cutting edges of tools of a known diameter, surprisingly high accuracy can be achieved straight off the dial

Click to expand...

Something like this?

wesg said:

Something like this?

View attachment 286482

Click to expand...

That's right, just make sure you can take small bites, ………...oh and leave it a little bit over length so you can face off any chipping from tool break out

Does it have to be acetal? That would be a reasonably easy part to do a silicone mold and cast it out of Task 9 or whatever material is suitable.

Conrad Hoffman said:

Does it have to be acetal? That would be a reasonably easy part to do a silicone mold and cast it out of Task 9 or whatever material is suitable.

Click to expand...

I considered making up a simple mold for it, but I don't have anything castable on hand. That steered me towards a form broach, and when it didn't work out, I figured I'd run it by here to see if there was something simple I'd missed or could improve to get a better result. Lots of good ideas here, I'm confident that I will be able to find some combination of these suggestions that will work!

Broaching will work just fine. You need to make your broach much longer and with a much better finish and very very sharp, Your tearing the material not cutting it.

Hi All:
I agree with pretty much everything that has been said in this thread but the comments of SIP6A are particularly relevant to why it didn't work in my opinion.
Your failure was not one of principle; it was one of execution when you made the broach.
You need to make a better broach (and you need to support the OD well too as several posters have mentioned)

So what resources do you have in house to make a better broach?
Do you have a T&C or surface grinder?
If you don't you will likely fight half of forever to get a decent result, and if that is so, I'd bite the bitter pill and follow TeachMePlease's advice.

Making two simpler broaches is a good option if making the complete profile accurately in one is going to be a major fight, but then you need to have a reliable way to index them and the second broach needs to be prevented from drifting if the cutting forces are not balanced around the periphery.
Since making a multi toothed broach properly raked and relieved will be harder to do, I'd also consider making a few single tooth broaches of increasing size and run them in succession if you are only making a few parts.
If you do it that way, it will be all about how easily you can index them accurately, each relative to the last and how well you can keep them from drifting.

Cheers

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

BoxcarPete said:

I have no doubts of that. Unfortunately, I don't think the budget for this project can support a custom-engineered tool from an outside source for just a couple pieces. I was planning to use the down time from the current slowdown to make it happen. I am prepared to do some hand-fitting, but my first attempt was a bit too far off the mark.

Click to expand...

Just for curiosity's sake, send him an email and ask for a quote. I bet it's less than $60 shipped (This is just a guess as my broaches are much smaller, but they're usually around the $20 mark)

Any reason not to rotary broach it inside a sleeve with a internal bottom lip? If you made a push broach you should be able to make a rotary broach as well. maybe slit the sleeve for easier removal.
Bill D.
Rotary broaches, not just for hexes any more.

TeachMePlease said:

Just for curiosity's sake, send him an email and ask for a quote. I bet it's less than $60 shipped (This is just a guess as my broaches are much smaller, but they're usually around the $20 mark)

Click to expand...

That's a lot more affordable than I expected. I think I'll have one more go at making my own, and then maybe go that route.

I'll probably make two, each one with half the step size. I tried a simple hole enlargement broach with the original one I made after knocking off all the burrs and honing it (probably could have used quite a bit more, but I did some), and it gave quite a good result. So, I suspect that the damage done to the broach when holding it for the mill ops and its new asymmetrical shape unbalancing forces are contributing to the poor result.

I'll post some updates here when I get a usable part.

Don't broach this. It's delrin, you can set your lathe up as a slotter. You may need to do some fancy fixturing to index the
spindle but a single point tool will do this easy. Take a few thou depth of cut.

Other choice would be an indexing head on a bridgeport, set vertical, again used as a slotter.