What's new
What's new

Using a bull nose EM to break edge with live tools.

Captdave

Titanium
Joined
Sep 24, 2006
Location
Atlanta, GA
This afternoon I setup a small turning job that gets a milled 9/16" wrench hex cut with a 1/2" .060" bull EM to blend it into the 5/8" stock behind 1" of M12 threads. Ran a few parts before I left the shop but after diner got to thinking of a quick way to break the sharp edge.

So here is my thought and tell me where I'm going wrong. I should be able to copy the same milling cycle process used to cut the hex and change the EM size to .440" and go .030" or .040" deeper in Z to get the EM to just kiss the part to break the sharp edge. Of course I haven't check any of my numbers yet but off the top of my head I think it's doable.

I could use a chamfer tool in a radial live tool but have a couple of hundred to make and trying to avoid another tool change if I can get away without it, besides I have another similar job coming up soon in the same family that's 1-1/2" bar and 3,000+ of them to make so anything I can do to keep the cycle time down will help tremendously.


SQT15M T+
 
Have your tool grinder grind a chamfer on your end mill at the correct height. Then you can do that whole thing in one shot. Little things like this save tons of time in production.
 
What a slick idea:D Have a bunch of EM that need sharpening, I'll have them do a couple and give it a try.

Thanks for the great tip.
 
Well I thought I could change the cutting size of the EM by using the slot width but that didn't change the tool path at all. Just a brief look through the programing manual and it looks like I can have only one offset for that tool in Mazatrol.

Anyone else have an idea?
 
Well I thought I could change the cutting size of the EM by using the slot width but that didn't change the tool path at all. Just a brief look through the programing manual and it looks like I can have only one offset for that tool in Mazatrol.

Anyone else have an idea?

Slot width is mainly for graphics. Tool diameter on the Tool Data page controls the actual cut path--similar to how the turning tools use the tool nose radius value to compensate correct tool path.

Copy the process and just run the finish tool. You will need to alter the X and Z values to cut the second feature (chamfer).

Alternate method is to use the second set of X and Z wear offsets (not diameter comp). On my T-3 control for example, I would use tool 15-1 to finish the hex and tool 15-2 (-2 is second offset value for tool 15) and adjust the wear values X0.080, Z-.04 for example.
 
Copy the process and just run the finish tool. You will need to alter the X and Z values to cut the second feature (chamfer).

We did that and he is running the parts now, I looked for a second set of offsets for the same tool but I thought Mazatrol only allowed one offset per tool as I didn't see a way to describe it as you mentioned. Of course that would be in the only book I'm missing for this control:willy_nilly:

Looked again and I'm not seeing a way to do as you mentioned. If you get a minute and could post a couple of screen shots that would be swell.
 
Last edited:
We did that and he is running the parts now, I looked for a second set of offsets for the same tool but I thought Mazatrol only allowed one offset per tool as I didn't see a way to describe it as you mentioned. Of course that would be in the only book I'm missing for this control:willy_nilly:

Looked again and I'm not seeing a way to do as you mentioned. If you get a minute and could post a couple of screen shots that would be swell.
If you post a screen shot of your tool offset wear page and a second pic showing the milling PNo process, I will show you what to change on your machine. Mine is a bit older and some stuff is different, so I do not wish to confuse you.

Mazatrol only allows one offset per tool on the same process--not per tool. Second process copied with same tool can use an alternate tool offset.
 

Crap. Now I feel like a liar. :leaving:

I will post a screen shot of the tool offset page on my T-3 later.

Here is a screen shot of a program when I was using a .094" wide Top Notch face groove tool. Tool 8 is described as GNL EDG 3°,0° R0.007 and NOT a groove tool. I was driving both sides of the tool. Tool 8-1 is probed as an ID tool and has about .002" wear offset. Tool 8-2 is driving the tool as an OD tool and the X wear offset on tool 8-2 is slightly different to control the OD tolerance on the groove separate from the ID on previous process.
 

Attachments

  • Mazak T_3 tool 8 dual offset.JPG
    Mazak T_3 tool 8 dual offset.JPG
    82.5 KB · Views: 2,316
All I can add to the tool in the PNo is a code (A-H with soft keys) which from what I can tell doesn't mean squat as far as offset goes.
 
All I can add to the tool in the PNo is a code (A-H with soft keys) which from what I can tell doesn't mean squat as far as offset goes.

There's your answer! :D

Again, I have never ran a T32 control, but on the T+ control on the Integrex 35 we used to have, you could 'insert' a tool line into the Tool Data 2 page.

Each tool was called up as 22V or 22H (horizontal position or vertical position) as this older Integrex had a turret that flopped back and forth. I could insert an additional tool for tool 22 in horizontal position, but designate it 22B (or something like that).

This will require you to add all the tool data into the machine as if it was a totally new tool and have completely separate tool geometry for it as well.
 

Attachments

  • T32_3 Insert Tool on Tool Data Page.JPG
    T32_3 Insert Tool on Tool Data Page.JPG
    58.6 KB · Views: 1,356






Finished up those other parts so jumped on this while the machine was open. The addition of the "A" to tool 11 worked really nice, the only odd thing is the end mill stops rotating between 11 and 11A no big deal just thought it was strange.

Thanks for your time and knowledge, it sure beats plotting out a second set of points in CAD and programing a second PNo.

BTW, it took if few minutes to see that all I needed to do was use the insert soft key to add another tool in the setup page:willy_nilly:
 
Have your tool grinder grind a chamfer on your end mill at the correct height. Then you can do that whole thing in one shot. Little things like this save tons of time in production.

Needed to run another batch of 1,200 of these stupid studs so took your advise and had a couple of custom tools ground to cut the chamfer on the leading edge of hex and the radius blend in the OD.

Works very nice and the time savings (~8 seconds) over 1,200 pieces really does add up quickly. :eek:

Thanks again for for the great tip.
 








 
Back
Top