What's new
What's new

Economic in process Broaching options

Fal Grunt

Titanium
Joined
Aug 5, 2010
Location
Medina OH
I have a part that has a .169” square thru hole that is about .100” thick. Material is likely going to be 4140 cr ann.

Considering making a single point style tool to clean up the corners. Not sure what other options might be available. Any recommendations? Something inserted that could be used on other jobs in the future would be great.

Order is only 10 pcs, and I’m budgeting about $250 for tooling for this aspect in the quote.
 
Mill it with as small of an endmill as possible and broach the corners out. Not sure what you mean "single point style tool". I would use a square broach make from a HSS lathe tool bit or hardened drill blank. Shouldn't be difficult. Or for wire EDM , that is an easy job.
 
We made a home made one out of a carbide blank. 1/4" shank, .070" square broach. Grind a flat on the shank when grinding one side, then use M19 R/P for orientation (haas control, don't know if brother is the same) to lock the spindle.
This was brass material to be fair, not sure how it would hold up on steel. We also mill it out with 1/32" endmill so not much material left.
 
Already been said, but I've modified HSS blanks before, just to take a few corners out.

I've also made broaches out of 17-4. Doesn't need to be a fancy full length
broach, just a couple of teeth to take the corners out. Usually take it to
an H900.

For 10 parts 100 thou thick, you can get by with just about anything. Even
a prehard 4140 would probably get you through the job. Get her to size, and
then hack some teeth in there with a die grinder or a cut off wheel on a dremel.
 
PolygonSolutions.com

We use him all the time. I'm pretty sure the last broach I bought from him was under $25 and delivered the next day (he's local to me) even though it was a custom size that he made from scratch. He'll do onesy twosey quantities without complaint or upcharge.

If orientation of the broach isn't an issue, you could rotary broach them, which will go much quicker, IMO. The rotary broach holder from polygon would set you back about your tooling budget by itself, but would be usable for all your future broaching jobs, so might be worth it to you in the long run.
 
Mill it with as small of an endmill as possible and broach the corners out. Not sure what you mean "single point style tool". I would use a square broach make from a HSS lathe tool bit or hardened drill blank. Shouldn't be difficult. Or for wire EDM , that is an easy job.

By single point I mean more like a lathe tool, and less like a broach. Last place I worked with broaches, a broach was a 8-10ft ground tool with hundreds of teeth :D

I considered wire, but everywhere around me, even on "low precision" jobs, is too expensive. Most wire shops I know are running at capacity and are adding more capacity. Lead time would be 6-8 weeks from any of the local wire guys and if I setup the Brother, I have other jobs that would benefit, I would learn something.

HASSAY SAVAGE CO. Square Broach, Fractional Inch, 3'/'16" Square Size - 12V319'|'14012 - Grainger

Just a simple square broach is a 4 hour cost to justify part... and still you have to grind it to your size.

starting with a 3/16 lathe bit a surface grinder hand could make one in an hour but it a little short of length....likely need two tool bit lengths to make drill hole size to square.

QT RJT: [Or for wire EDM ] there a good idea.
I've made a few broaches and I do make some specialized tooling for jobs, but anymore I just don't want to. If I can buy it for a reasonable price, I would rather buy it. Focus on what I am good at. I have one tool I make in house, I was quoted something like $500 for the the tool, and that was a qty of them, I made them in house, at something like $350-$400.

These are nice Broaching >> Horn USA, Inc. - EXCELLENCE IN TECHNOLOGY

You can pretty easily go 300 IPM. A spindle stop is required.

Danke!

We made a home made one out of a carbide blank. 1/4" shank, .070" square broach. Grind a flat on the shank when grinding one side, then use M19 R/P for orientation (haas control, don't know if brother is the same) to lock the spindle.
This was brass material to be fair, not sure how it would hold up on steel. We also mill it out with 1/32" endmill so not much material left.

Brothers spindles are a servo so they can increment by some crazy .1 degree. Over my head.

Already been said, but I've modified HSS blanks before, just to take a few corners out.

I've also made broaches out of 17-4. Doesn't need to be a fancy full length
broach, just a couple of teeth to take the corners out. Usually take it to
an H900.

For 10 parts 100 thou thick, you can get by with just about anything. Even
a prehard 4140 would probably get you through the job. Get her to size, and
then hack some teeth in there with a die grinder or a cut off wheel on a dremel.
I thought about making one, I have a lot of A2 laying around, but I think it is a good opportunity to add capacity to the shop. I still use my shaper when needed to clean up slots, and honestly, I have this nice new capable machine, I am trying to use 2020 to explore its full capacities and get the most of it.

PolygonSolutions.com

We use him all the time. I'm pretty sure the last broach I bought from him was under $25 and delivered the next day (he's local to me) even though it was a custom size that he made from scratch. He'll do onesy twosey quantities without complaint or upcharge.

If orientation of the broach isn't an issue, you could rotary broach them, which will go much quicker, IMO. The rotary broach holder from polygon would set you back about your tooling budget by itself, but would be usable for all your future broaching jobs, so might be worth it to you in the long run.

Thanks for that, I will keep them in mind, I have a job I was considering that a rotary broach may be the ticket.

Unfortunately, this job, the square locates the part, which times its function. So it must be precision broached.
 
I have a client that makes high end hand tools. He broaches 3/8 and 1/2 square corners in tool steel regularly. I believe he uses off the shelf rotary broach bits but holds them in a standard holder because of timing issue. You can M19 with an R to adjust the timing of the tool. I have also seen people fab up a lock system that locks the tool holder in position for keyways etc. Then you program with a drill peck cycle, spindle off, high speed chip breaker peck without full retract.
 
Thanks for that, I will keep them in mind, I have a job I was considering that a rotary broach may be the ticket.

Unfortunately, this job, the square locates the part, which times its function. So it must be precision broached.

Since you can orient your spindle, he will also make you a standard punch broach, for the same price and delivery.

Steve is the best broach supplier I've found yet, in terms of responsiveness and tooling quality.
 
Not yet, got the program written and did a dry run. Hoping to finish a job this week and then do the broaching job. Will definitely post when I do!
 
Square broach 3/16 down to your size , likely an hour to grind on a surface grinder..

3/16" Square Keyway Broach - USA | eBay


about .009 a side piece of cake.
I would grind it flat at taper. with a shim at mid section to be straight sided. Then dress SG wneel to 3* and bring each tooth to sharp edge. ..make about 4 finishers at .0002 under target size.

(Yes chek the existing clearance on the bought one and grind the same)

Grind the 4 finisher first straight at size, four sides. then set at taper to flat grind at taper, 4 sides. Then with 3* dressed wheel grind up to sharp.

If the broach is to long you turn around straight on the cross..dress the 3* the other way and finish sharpening. red dykem is best for seeing the clearance up to just sharp.
Only 6" long so no need to turn it.

New is only $126 so you might offer $100 for that usd one.
https://www.mscdirect.com/product/details/00307124
 
Well, this project took some mental aerobics to get up and running. Fun, definitely did not "make" money on it. But it was an excellent opportunity to LEARN. I am a bit embarrassed to admit I haven't done any "finger cam" since close to 10 years ago. Nearly everything I have run has been conversation, EIA, or I did the modeling and CAM.

I took raw, nearly worthless code from Fusion and hacked and slashed it until I got something that worked. Admittedly, there were some failures along the way, including breaking one of the $52 PH Horn inserts. :vomit: This was due to A being an idiot, and B not closely reviewing the Fusion code before expanding the code. When the insert broke, my rotation was correct(135*), but the face I was positioned over was the opposite. Fusion had X+ Y- instead of X- Y+.

So the cost break down works something like this.
I scored a $125 holder off ebay instead of $200. So that helped.
Inserts were $105 for two 5/32 inserts. I had to modify the back of them to fit into the hole.
$1000 of fiddle farting around figuring out how to do what I wanted to do.
3 months off my life due to the stress of intentionally running a non turning spindle into part.... intentionally.

I chickened out running the broaching tool. The recommended feed was 155 ipm. That scared the hell out of me. 30 ipm worked nicely. I don't mind plowing a big ass chip at mach chicken with my 1907 shaper that weighs almost as much as my S1000, but I just couldn't bring myself to run that high of a feed.

Code looked something like this:
(45 ROUGH)
G55
M09
M01
G100 G90 T20 X0.020 Y0.020 G43 Z0.77 H20 D20
M08
G00 X0.020 Y0.020
G00 Z0.77
G00 Z0.37
M19R45
G81 X0.020 Y0.020 Z-0.2092 R0.2 F30
X0.020 Y0.020
X0.022 Y0.022
X0.024 Y0.024
X0.026 Y0.026
X0.028 Y0.028
X0.030 Y0.030
G80
G00 Z0.77

I pecked out to the flat as my rough then after roughing all four faces came back and did the following finish cuts.

(45 FINISH)
G55
M09
M01
M19R45
M08
G00 X0.030 Y0.030
G00 Z0.77
G00 Z0.37
G81 X0.030 Y0.030 Z-0.2092 R0.2 F30
X0.028 Y0.032
X0.026 Y0.034
X0.032 Y0.028
X0.034 Y0.026
G80
G00 Z0.77

As you can see I took light cuts. It's Ann 4140, but I still didn't want to thump the spindle too hard. With only needing to make 10 pcs, the cycle time really wasn't an issue. With these cuts, there was no load, occasionally the Z would surpass the normal 4 green bars.

Something I learned that I am a bit ashamed I didn't know. M01 cancels all other M codes that are currently active. Who knew!

This was all a test for a small batch product that I am looking to make that currently gets broached with a tradition broach in a press. The broached feature is timed with other features in the part, and it would be nice to do it all in process to assure timing. And its faster, less handling, but DANG are the custom inserts expensive! Even when compared to a custom ground broach!

Hopefully Practical Machinist will allow me to get some pictures loaded up...
 








 
Back
Top