Surface finish problem

[Micromoldmaker]

I have uploaded file: dilator_el.mc9 to the /mc9 folder in the server. My problem is that when I try to get MC to spit out circular inerpolation to cut this shape, it gives me some unbeliavably raggedy surfaces. I've run into this in the past, and because of time constraints and not having access to this very cool forum, I just simply did it the "regular" way getting all G1 code.

In my file there's a toolpath for each approach. I wonder if somene can enlighten me.

[Midwest]

I think it might be your post. When I post your file I get G2 not G1.

 

Also try ramp instead of broken it will get rid of a possible line on your part because of the constant area of your z movements.

[Midwest]

Went back and looked at operation 2.......you don't have the filter on. Click on "total tolorance" and turn on the filter. Operation 2 outputs only G1's with my post. operation 3 uses G2's.

 

HTH

[Lee.]

I get Three lines of G2 and Two lines of G1.

 

If your machine can make Simultaneous XYZ moves then maybe change your settings to Follow Surface instead of Broken, it may get rid of your Lone Z move.

 

Otherwise the settings look good.

 

Try posting with MPMASTER bare bones post and see what you get.

 

Then go from there.

 

 

Let me know if I can help more.

[Micromoldmaker]

"Went back and looked at operation 2.......you don't have the filter on. Click on "total tolorance" and turn on the filter. Operation 2 outputs only G1's with my post. operation 3 uses G2's."

 

Midwest: Operation 2 is the one that works without gouges. Operation 3, the one that outputs circular interpolation is the one that gives me fits. I've run into this with 2 other machines, which made me think it was not a post problem. There seems to be something about round and near vertical surfaces.

BTW: the gouges only show up on the actual cut piece, never on verify.

 

Lee: I will try the MPMASTER post.

[Lee.]

I just checked the last op also.

 

Thought seeing as it was the only one checked.

 

HTH

[crazy^millman]

When is the last tiem you had the machined serviced. A little test to run on any machine to see if it is holding tolerence when cutting 3d. I got this from a service tech. Write a loop program to travel a 2" distance in X,Y,Z can be going in negatvie or can go in postive I write mine to do both but then run the loop at your normal cutting feed if they change alot you are having problems with the machine. I would also check my back lash to see that it is not out of tolerence and I would check to see you are not getting data starvartion on that machine we had a machine where someone hcnaged the buffere to line output and it gave us a fit till it got fixed.

 

HTH

[Midwest]

Did you try ramp instead of broken????

[Micromoldmaker]

I just recut the piece after posting with MPMASTER. No problems at all. Any body know what that's about?

[Bruce Gibson]

Micro,

I have uploaded dilator_el_bg.mc9

Have a look. In alot of cases I use 2d swept

to finish a "pin" like this. It gives very small code, and if you post it out, you will not see any

tiny linear moves as the filter will try to do as it "fits" arcs within your tolerance settings.

There are a couple of other ways to finish this shape, with possibly better lead-in/lead-outs.

jm2c

Bruce

[Micromoldmaker]

Well: I just recut the piece after posting with my usual post processor. It looks like moon craters on the tapered surface; the vertical diameter looks fine. I'm going to have a look between my post and MPMASTER, and if I can't find anything I'll check with my dealer. There's got to be something that's affecting the way the machine cuts; and I've run into this with 3 different machines in the past- definetely not a machine problem.

Thanks for your help, Bruce. The 2d swept looks really good. I think I'll start using some of the older toolpaths (I started with MC v7; there seem to be some really narly stuff there.

[Lee.]

Send me your post and the MPMASTER that you used, I'll take a look.

 

e-mail me.

[Micromoldmaker]

Here's the problem: arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R My post was set to 2 = R so it was not outputting I and J values, just R values. It's cutting just fine now.

 

Thanks everyone for their help.

[Roger Peterson]

I wish I would have seen this post right away, could have saved you some time. Been there. R values are notorious for this, always use I, J, and K's. With R values your controller has way too much control over the center point of an arc to cut it accurately. When cutting a contour you wouldn't even notice it but arc's that are very close in radius cut as close together as they are in a surface finish toolpath are not going to look good.

 

 

HTH