Anyone know if the Trim tool path will work on a drilling operation?

[Scott Lundin Shopware Inc.]

Wondering if the trim toolpath routine can be used to trim the Z depths to the tapered bottom surface of a block? In other words keep the path in Z only within the orange chain in my attached file. I tried a few things with no success. Any ideas specifically for the trim path? I know we could project the points down to the surface and pick them as incremental depths but was wondering about the trim path.

DRILTRM.MCX-7

[crazy^millman]

Scott could you save the geometry to a level. Then do a 3D contour toolpath. Use the trim tool to trim those operations to the surfaces or features. Use those lines to then make your drill point from. A little bit of work, but might save you time to drill the holes.

[Scott Lundin Shopware Inc.]

Ron that is a possibility as are others. I am just trying to nail down a definitive answer on whether or not the trim toolpath works on a drilling operation. Like I said earlier I have not been able to get it to do it.

[Thad]

Can't get it to work here either, Scott. It's interesting though since you can trim a milling toolpath from the front or side plane. Maybe because it's a canned cycle?

 

Thad

[?Mark]

Interesting. I thought I was able to do that few years back when I used drilling toolpath to drive my plunging tools...

[Lord Wukits]

Soooooooooo......

I've run into this as well. Is it safe to assume that MC lacks the functionality to trim a drill operation? 

[Colin Gilchrist]

I would say that is safe to assume. The motion you see on your screen is not a "line" it is the display that Mastercam creates, using the point data from the drill operation as an input. There is absolutely nothing to "trim".

 

Instead, go into the the view you are drilling from, take whatever surface forms the bottom of your part, and "project" the drill point geometry to that surface. Then inside the Drill operation itself, set your depth to "incremental" and set your top of stock to the normal start of drill cycle.

[taperlength]

It's like the OP said, just project the drill points to a surface and then drill incrementally to those points

[jlw™]

I wouldn't think  you could use trim on a drill path unless you're outputting longhand.  Otherwise your G81/G83 will all go to the same depth or either have to ouput multiple G81/G83 fixed cycles.

 

However, I have used what Ron is talking about to finagle some things in a CY lathe.  Don't see why it wouldn't work with a drill.

[Lord Wukits]

I wouldn't normally have to deal with this, but currently I'm on cabinet shop projects. As such I am using the trim on a transform operation to avoid a huge knot in the wood. 

[Pilot Plant Supervisor]

In G81 or G83 you can use X, Y, and Z. Not sure if the post will output that, but you certainly can program different Z's within the cycle.

[Teh Bear without Brains kinda idiot]

Trim toolpath is the very old way to do surface operations

It was used  when check surfaces and boundaries were not used or had limitied functionality.

It can be used for varios tricky situations but in most cases stay away from it.

And you will have lots of spare G0 movements  that trim is not able  to filter away.

I use Mastercam for 20 years and I  used it 2 or 3 times .

BR

[jlw™]

I may be old school but I use trim quite often. Pretty much all of my parts are and irregularly shaped. I'll use contour and trim more than facing. It's a useful tool.

[Guest]

I agree with the bear.....

 

for me, it's an absolute last option.......

[Mick]

I agree with the bear.....

 

for me, it's an absolute last option.......

 

Likewise. I exhaust all other avenues, and then when I do use Trim I think "ugh, I hate this toolpath"

[Mick]

Wondering if the trim toolpath routine can be used to trim the Z depths to the tapered bottom surface of a block? In other words keep the path in Z only within the orange chain in my attached file. I tried a few things with no success. Any ideas specifically for the trim path? I know we could project the points down to the surface and pick them as incremental depths but was wondering about the trim path.

 

Scott, I just looked at your file. The easiest way is just to project the points, and that is what I would do in the first instance. Many (many!) years ago I used to programme master blades for impellers, and I had to put spot marks around the perimeter of an impeller blade surface. Up to 300-400 points sometimes. I always projected the points and used incremental depth, and it worked perfectly.