Broaching in mill

[Rstewart]

I know this has been discussed before, but is the point toolpath my go-to for this operation?

I'm using 2021, haven't installed the update 1 yet.  Luckily I do have spindle orientation on this Haas.  

Just need to step in Y about .002 per pass, feed down, retract in Y-, then Rapid up in Z and repeat.  There's not a standard width broach for this application, so I'd like to be able to step over in X at Each depth cut.

Any pointers?

[JParis]

I wrote a macro for broaching but...

If I have to cut in XY at the same time, I draw a line out of the corner at 45° and place points as my steps along the line and step into the corner along that 45 

[JoshC]

here is an example of how i would do this. would probably need to manually edit the code some for the M19 etc.

 

https://fastechincorporated-my.sharepoint.com/:u:/g/personal/support_fastechinc_net/EXJl5Zoi2lpOhlh-F_founMBq1wSYydEOdMlenu9nVhvsA?e=9Ud8fm

[crazy^millman]

3D contour for the initial move then transform for the multi-passes you want to accomplish. Multi-pass got enhanced years ago and doesn't allow this to do it, but around X4 I was using Multipass to broach on lathes and Mills. 

If your machine has indexing in the mill spindle you can broach 4 places like I have in the sample. Would need to use a trigger to index and break up into separate operations. I did this on a DMU 80 and we broached 24 holes with 4 places each and when it was all said and done we held a .002 tolerance through al the holes and broaching operations. 

Here is a sample file: Sample File with broaching

[AMCNitro]

I did this back on version 7, yes version 7 not X7.  SO it can be done in 2021

[Rstewart]

My IT has my POS computer the rest of the day.  I won't get to experiment until tomorrow...

It is just a simple key slot 1.1" deep and .300" wide by .125 deep.  Through hole

[crazy^millman]

27 minutes ago, Rstewart said:

My IT has my POS computer the rest of the day.  I won't get to experiment until tomorrow...

It is just a simple key slot 1.1" deep and .300" wide by .125 deep.  Through hole

My example was a .25w x .125 deep x 1.0 in Z depth I have changed it to what I typed next stepping over in X+ and X-. You can easily use it to rough the center with a 1/4 wide tool then step over in X+ .025 and then X-.025. I would spread the wear evenly across the face of the broach verses doing one side then shifting to do the rest. If you can get a .300 wide broach made that would produce the best part.  

[htm01]

we had a broaching head on the hyperquadrex we had that was sweet ($15,000)

made a 10 minute broaching  about 15 seconds but we sold the machine

Mazak gave me a broaching program for for our integrex

[Rstewart]

Thanks Ron, I'll look into that to that tomorrow.  I would like to have a .300" broach made, time may not allow.  If I used a .156" it would be like cutting two keys next to each other?  

[crazy^millman]

1 hour ago, Rstewart said:

Thanks Ron, I'll look into that to that tomorrow.  I would like to have a .300" broach made, time may not allow.  If I used a .156" it would be like cutting two keys next to each other?  

I would do it the same way with roughing the center then stepping over in both directions. The .012 difference may not seem like a lot, but depending on the material might create a stress point in the material creating a crack down the road. By doing a center pass and then stepping out in both directions you give something for the broach to bite into. Where is .200 wide broach or something where you have at least a 70% overlap then I would say try it in 2 passes, but with a over 90% overlap just something I was taught to never attempt when broaching. I cannot point to anything more than my experience telling me to go about it this way. 

[Rstewart]

Ron,

Finally was able to check out your toolpath.  Very slick, I believe I'll use it.  

Thank you sir!

[Rstewart]

25 minutes ago, ONLYBLM said:

Me use wireframe ruled.

Is this pro_grammer ^

[crazy^millman]

1 hour ago, Rstewart said:

Ron,

Finally was able to check out your toolpath.  Very slick, I believe I'll use it.  

Thank you sir!

No problem sir and glad it was helpful. Have a good day. 

[88Matt]

Try the little used plunge mill path.