What mastercam toolpaths...

[sharles]

We are a mold shop and customers keep giving us deeper and steeper parts to make, and our CNC supervisor would like for me to be able to drop over a steep wall with a short tool and mill down the wall so far with that tool and then make a second program with a longer tool that would pick up where the first one stopped and continue down the wall. Is there a pair of toolpaths that work together to do that? The Z limit function really isn't a good option because often the steep wall is on a slope and so what would be a good Z limit at one part of the steep area wouldn't even cut the steep wall further along the contour.

 

If anyone could point me in the right direction, I'd appreciate it. I don't use the surface high speed toolpaths much. Is there something in there that would help? I know I could create surfaces to limit how low the shorter tool would drop over the steep wall, but then how would the second toolpath know where to start without starting back up at the top of the wall?

 

Thanks for any suggestions.

 

Scott

[Thee Rickster ™]

That is what I do.

 

I also do a roughing package with all Bullmills and then a finis package

 

Lets say.....I send a 4" stick out cutter down 3-3/4" the that is exactly where I start my longer

cutter at(with reduced feeds and speed of course for chatter and deflection)

 

I also make a surface at that level in case I use a scallop or hybrid using containment boundaries.

(as not to cut too much air on a cavity)

 

if i have 1 deg (minimum) draft then i use custom make drafted or tapered diesink cutters

[Jeremy Herron@DBS Solutions™]

I am not really understanding why you could not use the steep/shallow in the 3d highspeed or the cut depths option in the legacy toolpaths. Can you post a pic?

[Redfire427]

There is a Mastercam c-hook called "check holder" which I think is what you are looking for. It is supposed to allow you to machine different regions based on stick-out and toolholder clearance and then the toolpath can be broken up in different tools with the same description, but different stick-out amounts. I've personally never had much success with it, however, maybe you have some more patience and time than myself.

 

Carmen

[Guest]

Have you tried using depths to control how deep each tool goes?

 

Machine between 0 & -2

new OP, between -2 and -3.5

new op between -3.5 & -4

[Jeremy Herron@DBS Solutions™]

^^^ this is exactly how I do it ^^^

[sharles]

Thanks for everyone's replies.

 

JP, though I use Z-limit of depth a lot, it doesn't work when my part contour is tipped on an angle.

 

Jeremey,

 

I'm not very familiar with the 3d highspeed toolpaths (except rest re-rough). I put a picture in the ftp site "all pictures" folder called "scott steep walls". The area on the front right of the picture is about 7" deep, 3 degree draft, and P20 steel. You can see (hopefull) how the top of the wall is NOT flat. So the CNC sup would like me to be able to go about 3-4" down from the top of the wall all around the contour. I know I can make a limiting surface 3-4" down and that would serve fine for the "short tool" program. But how do I tell the long tool to NOT recut everything the short tool program did?

 

Rickster, can you explain more??

 

I wonder if my answer is in the high feed suite of toolpaths, but I know so little about them. Is there a good tutorial anywhere to help me understand their abilities?

 

Thanks Carmen,

 

I know our powermill guys do a lot with drawing their tool holders. Maybe sometime I will check into that.

 

Thanks for all the responses so far!!

[Cannon]

You can use holder checking in 3d high speed toolpaths, just measure the tool and draw the holder and put the amount you want the holder to be off from your part. Then make new operation with a longer tools and use dept limits or restrough

[Guest]

But how do I tell the long tool to NOT recut everything the short tool program did?

 

Rest with a depth.

[Cannon]

But how do I tell the long tool to NOT recut everything the short tool program did?

Save stl of the verified path with a shorter tool (or use stock model), and use that as your restroughing stock with the longer tool.

[sharles]

Is rest roughing the ONLY high speed toolpath that can do that? It's the only high speed toolpath I use (and I use it a lot), but my parts are pretty big and verify seems to crash on me once I start running finish programs on it so it limits my ability to create an .stl file for anything but roughing programs. Is there a work around to the limits of verify or do I have my settings wrong?

 

Scott

[Guest]

Loosen your stl tolerances up, I run at .003 as a default.

 

If I get a crash I open it up to .016, I keep opening until I get what I need.

 

You really should have a good enough handle on your settings that "look" isn't all that big, you're more or less looking for gouges

[sharles]

Thanks John,

 

I changed my verify default to what you said. I hope that helps. Thanks for everyone's suggestions. It gives me a place to start.

 

Scott

[Jeremy Herron@DBS Solutions™]

You have mail.

[Todd Tracey from Fastech]

Remember he's still running X4 guys

[sharles]

Thanks, Jeremy, and thanks for the reminder Todd.

[TERRYH]

Yea that probably limits us alot, is that we are still using MCX4, I work with Scott. Supposidly once we slow down they are going to look into some advanced trainning for us and alow us to upgrade to x5 or x6 so that we have more options as to how we do stuff. Every time we have upgraded in the past we go through all the pains of getting our posts back to how we need them as we use severl diffrent ones for the various machines we have.