What's new
What's new

Economical low cost broaching Solution

Fal Grunt

Titanium
Joined
Aug 5, 2010
Location
Medina OH
I have a part I am quoting that has a small through hole, 6mm (.236), that is a D shape. The flat is approximately .025" of the diameter. The depth of the hole is approximately 3/4", and it is a through hole. The flat orients the mating part. 4140 ann, approximately 150 pcs.

I plan to drill 3/16, then using a 1/8" high feed mill clean out the pocket to shape, leaving the 1/16r in the corners.

I was originally going to have the hole sinker EDM'd as it would be fairly cheap in regards to the electrode. A friend of mine suggested wire edm, but from EDM work I've had done recently, I would think that quite expensive (guesstimating $15-20 a hole based on recent work). I had considered a traditional broach, but the cost of having a custom broach made was a pretty high (similar part geometry quote was over $800 several years ago). I had a similar design/size part single point broach quoted by PH Horn, but the price was high due to the qty required (Approx $1400). Might be able to get a cheaper single point made from somewhere else.

I'm hoping you guys can give some input as to other options, or maybe you know other suppliers that I do not know because of locality or I didn't find them on the internet.
 
I would at least ping Ohio Broach and see if they might already have the size/profile that you need, and they could pop them in for you.


------------------

I am Ox and I approve this here post!
 
I have done D shaped holes in the past by milling as you described. You can avoid the milled radius the the corners of the flat if you predrill a hole at each end of the flat- lay it out in cad to get the drilled holes to clear your endmill radius. Yea, you loose a bit of the flat, but it usually works ok- run it by your customer and see what they say.
 
Take a HSS endmill shank and spin it down with relief, and then grind a flat on it, also with relief. Easy to make, and should shape the D-hole pretty easy.
 
I wonder if the wire cost would be much different if you skipped the milling with the small em. Wouldn't most of the wire cost would be setup? If you could save the picking away with a small em maybe that would offset the wire cost.
 
I would at least ping Ohio Broach and see if they might already have the size/profile that you need, and they could pop them in for you.


------------------

I am Ox and I approve this here post!
They were on my list to contact. The last "low volume" job I had contacted them about they weren't interested in. Or at least... I assumed they were interested by their lack of response!

What does a single point broach for a d-hole look like?
I've seen two different versions, I would call full form and partial form. Full form has relief but for the cutting edge. The partial forms I have seen are the forms sandwiched together, cut one edge, move to the other, or one design that was quoted, you indexed 180.
I have done D shaped holes in the past by milling as you described. You can avoid the milled radius the the corners of the flat if you predrill a hole at each end of the flat- lay it out in cad to get the drilled holes to clear your endmill radius. Yea, you loose a bit of the flat, but it usually works ok- run it by your customer and see what they say.
Due to the size, I wouldn't be able to drill a clearance hole small enough to depth. (at least I wouldn't!)
Take a HSS endmill shank and spin it down with relief, and then grind a flat on it, also with relief. Easy to make, and should shape the D-hole pretty easy.
I had considered it, but my grinder has been down and I haven't been able to get it fixed, so I am, for the first time in my professional career, grinderless.
I wonder if the wire cost would be much different if you skipped the milling with the small em. Wouldn't most of the wire cost would be setup? If you could save the picking away with a small em maybe that would offset the wire cost.
Well... that is something to consider. I use a 1/8" high feed mill, 15200 rpm, 46ipm, ramping the form down in. It goes pretty quick. Problem being, if I turn the part, then have it EDM'd, then I have to locate off the EDM to correctly index everything else. I'd have to rethink my fixturing to include locating off the bore.

I was thinking broach in process, but might send the EDM work out to a couple places to see if I can get a better price.
 
Have you considered milling a piece of HSS to shape and broaching it with your spindle after you use the high-feed? Or sticking a tiny grinding wheel in your machine spindle and grinding your own broach? Only 150 pcs in 4140, might be worth it for such a short run?
 
Have you considered milling a piece of HSS to shape and broaching it with your spindle after you use the high-feed? Or sticking a tiny grinding wheel in your machine spindle and grinding your own broach? Only 150 pcs in 4140, might be worth it for such a short run?
I have considered making one, honestly making one from scratch would take more time (cost) than having one made. I know from experience hard milled cutting edges do not cut as well as ground. The issue is really the relief cuts more than anything.

I have looked at grinding in the Brother, but always avoided it as I don't have any sort of filtering. Would this really need filtering, probably not.... I'm paranoid and over protective!
 
Although it will take a couple of steps, you can first make a "below-center" pilot hole the same diameter as the width of the flat. Make/get a square broach the same width as the flat (cheaper/easier to find than a d-type broach) and broach a square hole at the flat. You can then mill out the larger circle. Depending on how tight of a corner you can mill, you will still have rounded corners where the flat meets the larger circle but if you pre-drill the corners using small diameter drills, the difference would be negligible for many cases.
 
I have considered making one, honestly making one from scratch would take more time (cost) than having one made. I know from experience hard milled cutting edges do not cut as well as ground. The issue is really the relief cuts more than anything.

I have looked at grinding in the Brother, but always avoided it as I don't have any sort of filtering. Would this really need filtering, probably not.... I'm paranoid and over protective!
Have you considered buying a chinese D-bit grinder? They cost a thousand bucks and are pretty useful. I use mine all the time for this sort of thing. I use it almost every week to neck down endmills. The thing has probably made it's money back several times over just with the necked down end mills, not to mention the convenience of having the exact reach you need right when you need it. It would only take half an hour to grind your broach out of a broken end mill and I'm honestly very bad and slow at using the machine. I would pick this option a thousand times over going to EDM. I would make a broach for use in the CNC and then indicate it in and run all the holes at once without doing a tool change so the orientation stays correct.
 
Have you considered buying a chinese D-bit grinder? They cost a thousand bucks and are pretty useful. I use mine all the time for this sort of thing. I use it almost every week to neck down endmills. The thing has probably made it's money back several times over just with the necked down end mills, not to mention the convenience of having the exact reach you need right when you need it. It would only take half an hour to grind your broach out of a broken end mill and I'm honestly very bad and slow at using the machine. I would pick this option a thousand times over going to EDM. I would make a broach for use in the CNC and then indicate it in and run all the holes at once without doing a tool change so the orientation stays correct.

Can you link to an example of the machine you're referring to?
 
Another way, if the part and your customer will allow it, is to drill a 6mm hole then mill a slot across one side. Drop a flat insert in the slot and fasten it in one of several ways.

The simplest and fastest way to fasten that flat insert may be soft solder. It just needs to not fall out, the geometry supplies all the strength of a single, solid piece.
 
You don't have a toolroom grinder?


-----------------

Think Snow Eh!
Ox
Just a surface grinder, but it's been out of service for awhile now. I need to tear the spindle apart and figure out what's going on.
I have had good luck with the broaches from these guys https://www.polygonsolutions.com/

They custom made me some square rotary broaches with a different corner radius within a day of ordering.
I was under the impression that you couldn't orient a rotary broach?
Although it will take a couple of steps, you can first make a "below-center" pilot hole the same diameter as the width of the flat. Make/get a square broach the same width as the flat (cheaper/easier to find than a d-type broach) and broach a square hole at the flat. You can then mill out the larger circle. Depending on how tight of a corner you can mill, you will still have rounded corners where the flat meets the larger circle but if you pre-drill the corners using small diameter drills, the difference would be negligible for many cases.
I looked at doing something similar, but the depth and diameter necessary for the clearance holes would be a extra challenge that I don't think I would want to take on. Drilling a 1mm or smaller hole 3/4" deep just doesn't sound like a good option!
Have you considered buying a chinese D-bit grinder? They cost a thousand bucks and are pretty useful. I use mine all the time for this sort of thing. I use it almost every week to neck down endmills. The thing has probably made it's money back several times over just with the necked down end mills, not to mention the convenience of having the exact reach you need right when you need it. It would only take half an hour to grind your broach out of a broken end mill and I'm honestly very bad and slow at using the machine. I would pick this option a thousand times over going to EDM. I would make a broach for use in the CNC and then indicate it in and run all the holes at once without doing a tool change so the orientation stays correct.
I haven't used one of those before, but have looked at a couple older versions. I am morally opposed to buying chinese unless I have no other option, so I might keep an eye out for a Gorton or Deckel. I'd be shocked if I could make a broach in 30 minutes!
Rotary broach.

They sell blanks, which are round.

Grind to 6mm with appropriate clearance angle.

Grind the flat.

Several people have recommended Rotary broaches, am I wrong in my understanding that you cannot rotary broach an oriented flat? I was also under the impression that rotary broaching required symmetric forms?
 
Per your "orient" question:

I posted this recently.

This is a clamp-on guide/yoke/whatever that I used on my broach to orient a hex within a part.
In my case, the shank stabbed into a bolt hole in my collet closer, but in your case, it could locate on a chuck jaw or ???

Not commercial built unit. After destroying a cpl commodity units, I took the time to build my own.
Have not taken out any bearings since.


With all that said tho - I just don't see trying to push a 3D through hole in one shot.
Not that I have ever tried it, but the shank of your tool will be getting downright small clear at the back doo to back-taper Clarence. Let alone pushing a 3/4" long chip? Seems a bad plan to me...

DSCN3540.JPG


--------------------

I am Ox and I approve this here post!
 








 
Back
Top