Export to neutral file? wireframe, surfaces, datum curves unselectable

[texaspete]

I need help with "file, save as, neutral. I have some datum curves that were created using datum > curve > project. I want to export the datum curves as neutral geometry. When I do a "file > save as > neutral and a new menu pop up that prompts me for a coordinate system. The export selection ex. wire frame edges, surfaces, datum curves and points are not selectable. Can anyone advise me on how to do this. The goal is this, I am resurfacing or rebuilding a part using 12 cross-section from the old part.
Thanks texaspete

 

[Hora]

Texaspete,

Export your geometry in STEP format. STEP is also a "neutral" format and you can choose your curves to be included. Why do you need a ".neu" file? You don't have the step license?

-Hora.

 

[texaspete]

Hora
I have flex II package. I have a class A surface from IGES that I want to rebuild and make parametric. I realize that I will need 2 files to do this. The first file is the IGES that I import. Then "Datum Curve Project" onto IGES surface. Save the file and then SAVE-AS (Neutralm, IGES, STEP) I realize the cross-section will not be parametric because the feature is listed as a "imported feature". This was my plan, first create 12 sections through desired surface via Datum > curve > project onto iges surface. Then do a "file - save as" neutral, (or STEP or IGES). Third, import (insert - data from file) into desire part. We now have an import feature with surface and datum curves. Clean up the import feature thru redefine and delete unwanted stuff. Then create surfaces through import feature datum curves via Create - surface - advance - variable swept blend. This is where the parametric comes in. When a revision happens; I go back to the file that has the 12 projected sections replace the import feature with new import feature and during "fail mode" reroute or redefine the surface to new datum curves. My first thought was accuracy. I don't know it STEP or IGES'ing out Datum curves was a good Idea. I am trying to build a techniquing for dealing with CRAP CATIA surfaces. I get a so-call class A and find .25 to .50 degrees of error on adjacent surfaces. I find thru gauss curvature dumple or "oil can effect" in surfaces, surface that fold back on itself. Back to my question, Does this sound like a effective technique. thanks Texaspete

 

[Hora]

Hi againg Texaspete,

Looks to me you really need the ATB bus interface. Probably you know about it. I don't know how it works with Wildfire (if is able to read CATIA 5 parts). The main advantage is that you can have a direct link with the CATIA part (or any other neutral file) and is able to update your design when you change those neutral parts.

I'm wondering in your case if is not possible to create the 12 sections as you did, but a little bit different.

1. Create a new part let's say MASTER.PRT (nothing there except default palanes and CSYS -optional this one). Import data using INSERT->DATA FROM FILE->choose your STEP file.

Create your section here using the projection or surface intersect with planes.

2. Create a new part let's say FINAL.PRT (same as the first one) and here use INSERT->SHARE DATA->COPY GEOMETRY FROM OTHER FILE-> and you can select your curves from the MASTER.PRT. Create your surfaces using the imported curves.

Now you have a link between these two parts and you don't need to clean up the unwanted geometry.

So far so good. The bad thing is that if your original CATIA part change and implicit the neutral file used to be imported in MASTER.PRT you'll have redefine the first feature of the MASTER.PRT (which is the import of the neutral file) and then to recreate the curves.

I don't know if this method will simplify your life, but give it a try. Try to avoid cleaning up the unwanted feature.

If not, then ATB bus can save you time but as far as I know this module is very expensive.

Good luck,
-Hora.

 

[texaspete]

Hora, Thanks for the your help. I am building on this experience. So far, the class A has not changed meaning that the first few features are good. Again - thanks best regards - texaspete