Need help with basic milling tool path

[YARGNAIRB]

I am having trouble finding the toolpath that I would like my mill to take for machining a particular part. Without a doubt, most of you can answer this for me in a lot shorter time than it is taking me to type this. However, I have litterally spent several hours now and can't figure this out... I am milling a part and basically need to leave a Trunion Stub (Pivot Pin) remaining from my stock. I've made several of this part already and have many more to go. But I want to change my Toolpath to one that would better suit my needs. From my bare stock/block, I want to Helicoil cut (slightly larger than my finished OD size) completely down at approx 2 deg angle to my total desired depth. Then I want to (at full depth) climb cut 2 finish passes, bringing my remaining "protruding pin" down to my finished OD size. Does that make sense? I've only been at MC for about 2 weeks now and have already learned a ton, but I can't for the life of me figure out how to make this toolpath happen. Any help with this, is GREATLY appreciated.

Thanks for reading,

Brian

[DavidJackson]

2d contour

ramp+angle

multipasses - machine finish passes at final depth

[Colin Gilchrist]

I would make it in 2 separate toolpaths. I would use Contour, set your Contour type drop down box to "Ramp". This will let you put in your 2 degree angle.

 

Do not use finish passes (they will be ramped too), but set the "Stock to leave" to the thickness of your two passes. So if you want to take 2 .01 finish passes, you should enter .02 in stock to leave.

 

Now create a 2nd Contour toolpath at full depth that just cuts your finish passes.

 

This is better because you can also change the feeds and speeds. Run slightly aggressive feeds on the ramp, then slow it down for the finish passes.

 

If you need cutter compensation, you can also leave it off for the ramp, then enable it for the finish passes with Lead In/Out.

 

There are some 2D High Speed toolpaths that *might* do something close to what you are asking for, but you would have to create and manipulate multiple boundaries...

[DavidJackson]

^ agree with the rest, but what do you mean by the (full depth) finish pass will also be ramped?

[Colin Gilchrist]

Nope, I was wrong. I had multiple rough passes turned on, not multiple finish... my bad.

[DavidJackson]

You had me repeating it over and over trying too see what i was doing wrong

[YARGNAIRB]

I'm thinking more along the lines of what Colin is talking about by using the 2 separate toolpaths. I'm going to give that a shot now. Thank you guys VERY MUCH!!!

[Colin Gilchrist]

Sure, glad we could help.

 

The only way I could get it to not retract was to turn off all lead In/Out. That causes the cutter to retract up the wall at the end of the toolpath.

 

One trick that might help you here is to enter some distance in the "Overlap" data entry field in the Lead In/Out parameters. This overlap will spread out the entry/exit moves so that you get less of a 'dwell' mark where the cutter enters and exits the cut...

[YARGNAIRB]

WOW!!! You guys nailed it! And I learned something new! Thanks to both of you Colin & David. It's impossible to show you both my TRUE appreciation for your help, therefore all I can offer is my TRUE THANKS! Hopefully some day I can return the favor!

[Colin Gilchrist]

That's why we are all here man. Your thanks is enough. Glad we could help you out.

[Chri]

Hey Brian,

Making chips is fun, isn't it! Just curious, is the part in question the same pics you sent me? The ramp feature is one of my favorite things about MC. A lot of times I can program a part to cut to depth, using the lead in to remove most of the material. Example, 1" id bore @ 1.5" deep. I would use a .5 endmill, and use a contour ramp leaving .020 or so for finishing. The 3 degree ramp would clear all the material in the middle, step over and make the finish pass, and it's done. Instead of making 3 cuts at .5 DOC. I hope some of that made sense, Anyway, when are we getting together for lunch? I got something for you that I think you will like...

[Elmer Fudd]

If you would like to do this in one toolpath set your ramp motion to depth and check make pass at final depth. then set your multi passes 1 rough and 2 finish and check machine finish passes at final depth and check keep tool down.