EXPORTING SKETCH POINTS

[SolidCreative]

I have a component in catia with sketch points, or id points, where spot welds are going to be located. Is there any way to export that info with the model, or as a 3d sketch? Whenever I export I loss the sketch points. Im trying to bring it into solidworks, or MDT6

Thanks for any info anyone may have

Matthew

 

[rikman]

There is a roundabout way of getting the sketch points into 3D space in Catia V5.

1. In the Power Input field (the text box on the lower right of the V5 interface), type "t:vertex".

This will select all elements of type vertex (sketch points,"real" points, etc.).

2. Within GSD, select the project icon.

All the elements that have been selected in step 1 will now appear on the input list for this command.

3. Go through the input list and remove everything apart from the sketch points you are interested in.

4. Select the sketch definition plane as your support and click ok.

This will get you a group of 3D projection points equivalent to your original sketch points.

I know its a bit of a pain, but I haven't been able to get the search tool to pick up the elements in the way I'd like (it keeps selecting the sketch as a single entity and causing an equidistant element projection error).

Hope this helps

If Beethoven had been killed in a plane crash at the age of 22, it would have changed the history of music...
and of aviation.

 

[jackk]

Another way (maybe) would be to select the points inside the sketch, right-click and use OUTPUT FEATURE. This should 'expose' the points outside the sketch and make them available for export, just like ordinary points.

(I haven't tried it - so this is just theory)

 

[Camille1]

Yes, jackk is right, you can use OUTPUT FEATURE. Or another way to do it with VB scrip.

Dim PartDoc As PartDocument
Set PartDoc = CATIA.ActiveDocument

Dim GeoElements As GeometricElements
Set GeoElements = PartDoc.GeometricElements

Dim GeoElement As GeometricElement
For i = 1 To GeoElements.Count
If Instr(GeoElements.Item(i).Name, "Point") then
Set GeoElement = GeoElements.Item(i)
MsgBox GeoElement.Name
End if
Next