Proe mold model->SW->Step=faceted tool?

[Hein_]

Greetings,

My name is Hein and have only made a few posts here. I've modeled a few molds in Pro/E. I'm running ProE 2001 if that's any indication, Lately, I've been modeling molds for composite parts. Fun stuff. The molder uses SW2010 so I export Pro/E surface models (created at a high accuracy setting) via IGES to SW where I check and save files for him to verify my work.

He then sends those files (or occasionally STEP files created from them) out to a few different machine shops who then make the molds mostly using MasterCam (I believe). Most molds come out great but occasionally he gets faceted surfaces in his molds. I haven't seen all cases of this but it seems to be on larger radius surfaces that are more-or-less normal to the Z machining axis. below is a picture. This mold has been sanded slightly but you can clearly see the faceting. I actually feels smoother than it looks.

There isn't any finger pointing going on and the parts are coming out great! I just want to help him solve this.

As a side note: I am looking for a used horizontal or vertical machining center (~$15K) so I can start making a few molds. I currently have a large Multicam CNC router and I have not seen this when cutting large molds which I have modeled and programmed completely in Pro. I would like to say that this will not be a problem when I make molds but don't want to eat my words.

Any ideas?

Thank you.

Hein van Swaay
Impact, Inc
54I 49O 5O9B



Edited by: Hein_

 

[Hein_]

Maybe I should have posted this in Data Translation. Mods please move it if that seems appropriate.

 

[kshowdown]

I know in Pro/nc there is a tolerance setting default of .001. I set mine at .0002


the tolerance setting is for the maximum allowable deviation from model geometryin tool path.

 

[Hein_]

Thank you for your reply.

Does anyone know if there is such a setting in Master Cam?

So this has something to do with the interpolation of the tool path. Is that right?

Thanks,
Hein

 

[kshowdown]

circular interploation in pro/e is for changing the output of any given radius. Either points or arcs. usually older machines are points. This has no geometry control.


Master Scam should also have a tolerance setting.

 

[spaggioli]

Hein,


Mastercam does have such a setting but the faceting you are seeing could be caused by a lot of things, those settings only being one of them. Machining practices being another and original geometry being converted another. I would post your file if you can and we could take a look and possibly exclude the geometry.

 

[Hein_]

Here's a link to a zip file containing 4 files:

http://www.impact3d.com/surface.zip

surface_from_pro.igs = surface saved-as from original (design) model. (The surface in question is an extruded conic in the original model)

surface.sldprt = This part was created by saving a SW part that contained a surface offset=0 feature referencing the original imported (from Pro via iges) geometry.

surface_from_SW.STEP = save-as of surface.sldprt

surface_from_SW.IGS = save-as of surface.sldprt

I really appreciate you taking a look at these. I brought the surface_from_SW.iges back into Pro/E and it looked OK. Surfaces also look OK using zebra stripes in SW.

Could this also be caused by a post or machine controller?

Thanks
Hein

 

[kshowdown]

Hein


The surfaces are fine. They have nothing to do with your problem. If you go into Pro/e / view / display settings / model display / shade tab and change it to 1 and also go into the edge/line tab and change to low, you will get a crappy looking surface that will machine just fine if your machininig parameters are set up right.


I would also machine that surface at a 45 degree angle. also in pro/e I would put a .0003 scallop height and letthe software control the step over.


Good luck.



Edited by: kshowdown

 

[srieger]

I would not output the models as an Iges. If they are going to SolidWorks you are better off to export as a step from Pro/E or a Parasolids .x_t file. With these formats you will get a solid model as designed and not be exporting based on the display accuracy/resolution.

 

[Hein_]

Thanks for the replies and suggestions, everyone. I am still thinking this is a programming, post processing or controller issue. It looks to me a like the machine is not using enough arc or line segments to approximate the conic surface.

I'm no expert on G-code post processors or CNC machine control. Is it true that all trajectories are ultimately approximated by lines or arcs?

This is all very interesting to me since I am looking for a machine to make molds like this. I can't afford a new machine so I'm looking for ~10 year old machines but don't want to pick one with a limited controller.

What would be the preferred controller for a ~10 year old machine running molds like this?

Thanks,
Hein

 

[cedge]

Hi Hein


I believe you're right in assuming its an interpolation__g-post/controller/machine issue. If your surfaces are true surfaces (as in they are defined by formulas and not point to point or facetdata) they should result in a smooth finish. looking at your picture I'd say the surfaces where machined using linear interpolation.. (because the spacing is larger as the radius increases). This is driven by the G01 code with many points. It should be driven by the G06 (spline interpolation) code


I won't pretend to know much about cnc controllers as I am new to all this. I have recently come across the same problem while machining a cylinder. I was profiling using a helical motion so the expected it to use G2 intepolation but it used G01.. I'm not sure if its a wildfire 2 issue or the PP, maybe some one knows?


So, Perhaps the cnc machine's controller was not capable of spline interpolation and therefore was output as G01 or the post processor or cam software incorrectly output the code as linear point to point. Ask your machinist for the code


Hope this helps