Mastercam & Solidworks

[JonnyB]

Has anyone had any experience opening Solidworks files into mastercam directly? Files that contain lines and arc are working fine but anything contains a spline causes problems... the spline gets broken down into very small lines and cause rough "faceted" surfaces, and mating pieces wind up with very poor fitup after machining.

 

Ideas anyone?

[Toolfab]

What versions of each software are you running?

[Rob Peirolo CNC Software]

JohnnyB,

If you are 2-D machining the spline, have you tried breaking the spline into arcs?

We use it all the time for flowpaths in turbine housings and it works great.

Rob

[Toolfab]

Have you tried to save your SW part as an .sldprt file and use the parasolid converter in MC? That is what I use. I dont have any issues.

[JonnyB]

ToolFab:

I am using Solidworks 2004 Sp4.0

 

And for the4 mastercam I am not sure.. but I know that we use the latest stuff as a rule.. The NC guy is gone for the day so I'll have to ask him tomorrow... Currently we are saving the files as sldprt files... The next thing we will try is the parasolids...

 

Rob:

I dont have any way to break a spline into lines and arcs in Solidworks I can go the other way and take lines and arcs to splines just not the other way around... is that a MC command? If so I will have my NC guy look at it...

[Toolfab]

you are saving them as .sldprt's and still having issues?

[JonnyB]

Yes, Im saving them as native Solidworks documents, sldprt for parts and sldasm's from assemblies... we do have a parasolid translator as well that I know of and I will suggest that they try that...

 

what we are having problems with are the trim steels... we copy the edges of the design part and copy ("convert entities")the edges into a sketch for solidworks to extrude or cut. this leaves a nice smooth looking trimline when viewed in solidworks but after importing to MC they are short lined facted edges and faces.

[Toolfab]

can you put a sample on the FTP for us to look at? BTW,

 

 

welcome to the forum!!!

[Hardmill]

You may want to put up a sample on the ftp.

The guys can get a better idea of your problem

if they can actually see it.

BTW Welcome to the forum

 

PEACE

[JonnyB]

Yes I can put a solidworks part file up there, It will be there in a few minutes... I will provide a link when I get it there. I dont have access to the mastercam file though.

[JonnyB]

Oh and BTW thanks for the welcome!

[JonnyB]

Ok I have uploaded the SWX document under the path:

 

ftp://mastercam:[email protected]/Ma...lids/243.sldprt

 

let me know if you have any ideas... perhaps this is just some settings I need to address in MC?

 

Thanks again for all your help

[Toolfab]

Ok John, I have looked at it, and I may know what you are talking about now. I have put 243toolfab.MC9 in the solids folder, it is right under the one you put in there. What I did as you can see on level 3 is create arcs about your splines. I have found it hard to get good path off a spline so I create arc's. I was shown how to do this a while back hopefully this will help (thanks Jay).

 

Look at level three, let me know if this is what you need and let me know. Then I can explain how to do that. If not, let me know and we can try the next thing.

 

quote:

---

Thanks again for all your help

---

Help and be helped, that is what this place is about!!

 

[JonnyB]

Thanks PAul I will hand this off to the NC guy and see if it looks better to him. So what you're saying i take it, is that there really isnt any "setting" that I can tweak, its more of a manual function that needs to be done by the operator. Correct?

 

Thanks again

 

Jon

[Toolfab]

To the best of my knowledge there is no setting. You just create an arc about the spline.

 

Set your Z depth to the plane of the spline, create ard, 3 points. Then take one endpoint, then the midpoint, then the oposite endpoint.

 

With the file that you were using I had to break your spline into "many lines" because of the way it was drawn. Then you go from there. Create the arcs on the different splines, then trim them together and there you go. You will have a smooth true toolpath.

 

The hole process for your file took me about 3 minutes, after you become comfortable with it, it goes very quick.

 

[JonnyB]

Thanks again Paul.

 

I guess that really proves MY point though. They thought that it was my software not creating them correctly. I showed him your post and the MC9 file. So now he knows what he has to do then! My thing is that when I design a trim steel I must follow the customer part lines faithfully, and I have no room for interpretation. Although I must admit that I do add-lib sometimes when I know I can get away with it! Shhhh

 

Thanks again for all of your help!

[Charles Davis]

I would not break the spline in Mastercam. It will make further work on the part more difficult, and it simply is not necessary. Just set the Filter tolerance a little tighter.

 

Mastercam DOES filter properly (believe me, I've tested it extensively a while back, and it does exactly what you tell it to do). However, a .001 filter tolerance is clearly visible on the finished part! The part looks like a freaking disco ball. .001 is NOT enough.

 

I suggest you turn your total tolerance to .0002 to .0005, and make sure you are filtering for arcs, not just lines.

 

I hope this helps.

[JonnyB]

Yeap that what we are getting all right... we a male and a female trim steel being machined and they look just like that.. a faceted disco-ball!

 

I'll pass that along and see if that helps.. you know if I could get them to hook the NC guy up to the internet he could ask these things himself! LOL