3D contouring basics?

[Donkey Hotey]

Well, thanks to a number of people sending me information about my MC X post problem, I'm finally up and running. Thank you to all, for the outreach of assistance.

Now I'm up to making my first contoured parts. It's my first experience with ball-milling and I'm having some problems. I'm getting a grip on what the various options are in the dialogs but I'm still having problems with the edges of the surface.

Attached are two images. The part was designed in Catia V5. The 3D contoured area is the top of the ribs (seen in the finished part). I was able to get an export of the uncut upper surface from Catia (without the pocket holes).

Using that surface, I did a roughing operation that left about 0.040 on the part. After that, it was a circular finishing operation with 0.001" tolerances. I used a 3/4", 2 flute ball mill for all of this.

The problem can be seen on the edges of the surface (perimeter and at the top of the cone). I had to go into Advanced Settings and change the surface edge action to "Only between surfaces" to keep it from rolling over the edges. Now it looks like it's not quite making it to the edge at all.

With the defaults, the endmill would wrap over the edges. The result is that the mill would cut into the pocket at the top (which I didn't want) and off the outer edges (which would run into the vise).

What options should I have used so the ball mill cuts right to the edge, without plunging below the surface edges? If you look at the finished surface you can see the rough surface left at both boundaries.

BTW: I'm using MC X

Thanks in advance

Similar Threads:

• Need Help!- contouring
• Help with contouring
• 2d Contouring
• Help with 3D contouring
• contouring help

[fourperf]

wow greg, those are very impressive. at some point I want to get the license to run my cam program 3d (sw/camorks). Those parts look great.

Mark

[Donkey Hotey]

Thanks Mark. I'm kind of embarrassed that they are so simple and it's taken me this long to get here. All of that exercise to machine the upper surface, only to machine 95% of it away afterward.

The ribs could have really been designed differently but I figured this was a good time to tackle the contoured surfacing problem. I get a chance to evaluate the surfacing results before the pockets are cut. I have to make 24 of these so I also get to tune the settings and see the changes.

It's amazing to me that you can actually see the surface facets that Mastercam used for the cutter path. Look closely at the contoured part before pocketing: you'll see tiny triangles/diamonds reflecting back. They look bigger than they are. They'd probably come off with wet sandpaper and a polish--or another three hours in the machine with overlapping cutter paths.

[PBMW]

Greg
You can save a ton of cycle time by pocketing first and then doing the 3d stuff.

[Donkey Hotey]

That's true but this was a chance to experiment. I did it this way for a couple of reasons:

1. I wanted to learn about surface finish vs vs cycle time and the tolerance settings in MC. I get to make 24 of these so it's a chance to play with it a bit. If I have to make 25 or 35--no harm. The material came out of a scrap bin and they're just happy to get them.
2. I didn't want to rough the material off of those narrow ribs without support around them.
3. Mastercam kept breaking those ribs up into thousands of little herky-jerky moves. I have the high speed machining option on my VF-2 and I had not yet seen it run. It seemed more reasonable to keep the cutter moving smoothly around the part than doing thousands of little plunge-cut-retract cycles.
4. When I tried to machine just the rib caps, the endmill did the same rollover problem except it did it everywhere. It's like the ball wants to remain in contact with the edge of the surface all the way to the 90 degree point. This caused particular problems in the corners where the 3/4 ball mill would get shoved down into the 0.13 R pocket.

In my mind, the cutter path for the ball should 'stick' to the surface until the tangent point is passed. After that, it should release. Instead, the Mastercam maintains that tangency--as if it's a ball rolling off of a table edge and heading for the floor. It doesn't seem to let go until the ball has rolled all the way over the edge. That's what I'm trying to solve here.

[Matt@RFR]

Greg, for the outside profile, in the 'Finish Parameters' tabe (or whatever you have), click on the 'Cut Depths' button. Click absolute, then under maximum depth, enter the max depth you want the ball nose to run at. Make sure to select 'relative to' "tip". That should keep the endmill from rolling that corner.

For the top part, I think I'd try drawing a circle (or use existing geometry) to create a containment.

What's your email? I have a file that works (in verify atleast) of a VERY similar part...it's too big to attach here I think.

Uh oh, a student trying to help a student...this should get interesting.

[Geof]

.....It's amazing to me that you can actually see the surface facets that Mastercam used for the cutter path. Look closely at the contoured part before pocketing: you'll see tiny triangles/diamonds reflecting back. They look bigger than they are.....

Have you tried lightly dragging your finger tip or fingernail over these to see if you can feel them; it is likely that you can. Then dig into your CAM settings and you will find out how small the peaks are, this is the chordal height or something like that. (I think; I don't use CAM but have read a bit about this stuff.) As an example of how sensitive our sense of touch can be I find it interesting.

[Donkey Hotey]

Thanks for the responses, guys. It's not the part finish I'm worried about. If you look very closely at the round surface edge at the top of the part and the profile curve around the part, you'll see that there is a lip where the ball mill did the roughing but did not do a finish contour.

This is a ruled surface so it should be straight from boundry to boundry--ie: you should be able to lay a straight-edge across it with no deviation. In the photo, you can see a small cupped edge on both boundries. That's the problem.

[cadcam]

Greg go to advance setting at set to only roll between surfaces so the tool does not roll the edge.Can you share your file with me?

[Donkey Hotey]

Thanks Jay,

'Surface only' is exactly the setting I was using. I think it may have also had something to do with 'center' or 'tip' compensation. I changed it to 'center' and all of the paths were recalculated, above the surface at the cutter normal distance.

This makes more sense in my brain though I'm not entirely sure how 'tip' compensation works with a spherical cutter. 'Center' comp fixed the upper boundary (the circular one) but it still left a lip on the rectangular boundary.

In desperation, I made friends with the idea of creating 'check surfaces'. I put a ruled surface through the part, just above where the vise jaws will be and set that as a check surface. I also set the center, circular land as a check surface. Then I turned the 'roll' action back to automatic. Now it rolls off and finishes the edge, without running all the way down to the vise jaws.

Or at least that's how it looks in the simulation. I won't have a chance to re-run it until tomorrow but it looks great now on the screen.

Now I have to figure out how to set the dialog for peck, rigid-tapping. I've never rigid tapped on my machine so I'm going to jump right in with formed, 8-32 threads, 2.5-3 D in blind holes. What could possibly go wrong?

I'll post pictures when it's done.

[cadcam]

Four surfacing the normal is to let Mastercam calculate the Spherical tangency or the radii and this is done by tip.
I may missed some thing. But you should not have to make another surface for that part.
Looking at the order you did this in surface rough pocket then surface scallop.
Right to the edge.
Then pocket with additional finish path checked .roughing the pocket with the first pocket rough to floor only. Then the additional finish path pocket goes in and changed to a ball end mill for the radial walls. And finish.

This why I was asking to share your file so I could see how you did it the make changes and send back or make video to show.

Have fun Greg, sounds like you are.

[Donkey Hotey]

I may missed some thing. But you should not have to make another surface for that part.

The only additional surface I created was the flat, check-surface to limit the down-travel. But I'm still using 'center' comp. I'll change it to 'tip' and see how it does. I think with the check surfaces, it should be okay.

You're saying it shouldn't need the check surface?

Attached are the two results. It's a verification of only two operations: rough and finish of the surface. You can see how the cutter plunged through the hole in one example. That's what it was doing on the border in my previous cases. I can't duplicate it now but you get the idea.

Bad Tangency
Drive Surfaces only, tip compensation, Auto roll on surface edges

Good Tangency
Drive surfaces, check surfaces to limit edges, center compensation, Auto roll on surface edges

The stock size is identical between the two photos so you can see how far outboard the cutter is traveling. The fact that the cutter isn't traveling out to the edge is what's leaving the little lip on the perimeter.

I can email the file to you if we can't solve it this way (I lost your contact info though). Nothing secretive about it. I'm just trying to be minimal impact on your time.

[cadcam]

Thanks Greg I do thank you for this thought. (I'm just trying to be minimal impact on your time.)I try to help when I can.I for sure try not to ask if I cant find a few min to help.
I sent you a PM.

[cadcam]

Please review the start of the part you are working on.

Tried to make small for download.can change that later.Please turn on audio.

http://www.mastercam-cadcam.com/foot...footpart1.html

[Donkey Hotey]

Jay,

I can't thank you enough for doing that. I don't think your solution for the surface was any simpler than the one I came up with but I learned so many other shortcuts that your time and effort paid off in more ways that you know.

I'm still on MC X. I don't seem to have the Flowline options that show in your dialogs. But I didn't know that I could window-select everything and just set the boundary to stop at. I was going around clicking each surface. I also saw a bunch of other things. I'm going to go back and watch it a few more times to pick up some of your techniques.

You also kick-started me with the 'create geometry' options from the imported solid. With any luck I'll get to those parts tonight. I'm stumped with a Haas lathe problem right now.

Thanks again!

[cadcam]

So you know I would of not ruffed it this way in the shop for me.I use the rough pocket all the down in to the pocket to.
I also noticed on yours you never came down to the true surface to finish or was some of the finish missing.

Glad that helped jay.

[Donkey Hotey]

No, I thought the second surface machining operation did 'finish' the upper surface. It didn't? I'll have to go back and look at that.

As I posted in the beginning though: The intent was to leave the pocket material in there so the walls would have support during roughing. After the surface was defined, I'd step the pockets down in increments. The walls weren't high tolerance but I was trying to treat them as if they were (learning / practice).

[cadcam]

I thought the second surface machining operation did 'finish' the upper surface. It didn't? I'll have to go back and look at that.

Here is the info from your file.Review picture of STL compare.