How do I do broaching on a mill in mastercam?

[jpwmartin]

I need to do a broaching operation to the ID of a shaft on a mill, and I don't see any toolpaths in mastercam for broaching or slotting. I am using a Mazak VTC that has the ability to do spindle orientation.   How do I go about doing this?? 

[crazy^millman]

Point toolpath or a finish 3D contour toolpath will do it. The 3D contour give you the ability to back away from the wall with lead in and out. Point toolpath will do the same thing. Then do a Translate toolpath to control your step over and then you amount you need and good to go for the depth of the broach.

 

HTH

[jpwmartin]

Ahhh ok....   never thought of just using a 3d contour.... so do I just set the spindle speed at zero then?  And do I have to manually add in the M19 for orientation?

[crazy^millman]

Ahhh ok....   never thought of just using a 3d contour.... so do I just set the spindle speed at zero then?  And do I have to manually add in the M19 for orientation?

 

Just comes down to how you want to control it. Yes Spindle Speed Zero. I have done a mi trigger for the M19, I have done cantext or I have old schooled it and added it by hand.

[jpwmartin]

Ok good enough, that's awesome thanks so much for your help!

[The Cathedral]

Depending on what type of control you use, you're going to have to put a code in do do a feed move with zero spindle speed.

 

EDIT: I see you're using a Mazak; I don't know about those but you do have to on a Fanuc or Okuma.

[FROZEN]

Depending on what type of control you use, you're going to have to put a code in do do a feed move with zero spindle speed.

 

EDIT: I see you're using a Mazak; I don't know about those but you do have to on a Fanuc or Okuma.

You don't for a Makino

[mkd]

Depending on what type of control you use, you're going to have to put a code in do do a feed move with zero spindle speed.

 

EDIT: I see you're using a Mazak; I don't know about those but you do have to on a Fanuc or Okuma.

I'm going to need to do this on an Okuma macturn30. What code would enable feed without any spindle.

Thinking m110 indexed c axis of course, but no turret indexing as broach will already be indexed in lathe pocket.

[The Cathedral]

On our Okuma LT's with P200 / P300 controls, the code is M808 (cutting feed interlock release OFF) and then when you're done M809 turns it back on.

 

On our MA400HA horizontal mills with P100 controls it's M130. I'm not sure which one it will be since you're on a mill/turn; we have a couple Macturns and Multus' but I've not used that function on them so I don't know.

[Mr. M]

The Okuma Macturn will be the M808,M809 as well

[htm01]

check out PH Horn

 

http://www.hornusa.com/fileadmin/user_upload/usa/PDF/HORN-US-Chapters/KSTECH100IS_11.2011/KSTECH100US_11.2011_ChapterR_Theme-Broaching_Technical-Info.pdf