Inserting & Patterning Hole Features on a Curved Part. 1

[VN1981]

Hello,
I need to create fastener holes pattern on a curved part (wing skin panel) and I am having issues. First time trying to create a hole pattern on curved surfaces.

Since there are like hundred of holes, I decided to create a sketch with points and use the function User Pattern to pattern hole feature. In my prior usage, this approach has worked beautifully albeit most of the parts/components were flat surfaces.

Image below shows the 3 different sketches with points representing fastener hole center location.

I created the usual hole feature on skin surface as shown below.

But when I pattern them, things start to go awry.

Hopefully, this can be seen but somehow in one of the rows, the hole feature is not being drilled i.e. hole is present but it doesn't appear to have removed any material.

In another pattern, things are even more weird. As illustrated, Catia seems to be have created like half a hole?

Anyways, I understand in principle of parent hole feature drilling direction which in turn is based on surface normal and this could vary over the span of a curved surface and hence the weird outputs after patterning.

Is there a better way to achieve inserting holes on the skin panel? It is important that hole features are represented in the CAD model.

Would really apprecaite help on the above as it is kinda important that I find a way to accomplish the task.

Thanks in advance.

 

[LWolf]

2 questions:
Is the hole you are creating your pattern from defined as "up to next"?
Has your User-pattern "Keep Specifications" tick box active?

regards,
LWolf

 

[VN1981]

Hi LWolf,
It is defined up to last...I also tried blind option with sufficient depth. Still same issue persists!

AFAIK, Keep Specifications box was not ticked. I will have to recheck that part though.

Unless LWolf comes up with an alternative procedure, per my research so far, the above may not possible in Catia V5 using out-of-box command/option. Powercopy seems to be one procedure but I dunno how to automate it...else I will have to click 300+ times to make it work...plus I was not able to get the Hole feature to be included in Powercopy.

Yes on a simpler curved surface part, I did try creating a plane tangent to the point on a surface and the hole was generated on that plane along a line I created (normal to the plane+point). Still had issues including Hole feature in Powercopy.

Just surprised that Catia does not have a feature for software to make the holes tangent to the surface when even less sophisticated CAD packages offer the same.

 

[ferdo]

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[VN1981]

^^Thx for the reply Ferdo.

Beautiful! Is it possible to post a higher resolution of your Catia model tree or share your Cat part? Just curious to see how your were able to accomplish the above. I am having hard time making out the model tree from the above image.

 

[ferdo]

Is r24, is it OK?

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[Nigel P]

The ability to select 3D Points or Axis Systems is possible in V5 R2015 to do what you describe above.

The attached image shows a Hole (Up to Last) being replicated via the User Pattern function on a compound surface. The Yellow hole is the hole that is patterned; the Green holes are the ones generated by the pattern.

 

[ferdo]

True, I checked in R27 also and is possible by keeping specifications. I didn't check up to now...that's why is good to read what's new in new releases...



Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[itsmyjob]

@ Nigel P

does the axis of the hole keep the same direction or does it follow the normal of the surface? I have the feeling they all have same axis.

in order to have axis normal to surface we developed a script CAA but VBA or even EKL (knowledgePattern) would be better

Eric N.
indocti discant et ament meminisse periti ​

 

[ferdo]

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[VN1981]

Ferdo,
R24 is OK. Please do share the Cat part as I am interested in finding out how you achieved using Powercopy. I am still having issues with including Hole Feature in Powercopy.

Actually, as posted by Nigel P, I did play around with "keep specifications" option in pattern command and I was able to obtain satisfactory results for surfaces with high radius curvatures. However if the curvature varies severely, the output is not satisfactory even with Keep Specifications.

I will post pictures later if possible.

 

[LWolf]

Maybe this will help? it is a knowledge pattern... Delete all the udfs in OUTPUT_HOLES GeoSet, right klick on the Holes Calculation located in Relations-Holes Calculation Object, and do "Execute"...
basically put all your points into INPUTS-Instantiation Points GeoSet. Only the visible ones will be considered

regards,
LWolf

 

[VN1981]

Hi folks,
I tried to pattern a Hole on a highly curved part. I used Surface Normal in Hole definition box as well as "Keep Specifications" in User Pattern definition.

As one can see the result is not at all along expected lines.

The feature Hole.3 (left most one on -Y direction) is the original Hole feature.

Anyways, I think I've figured out on how to use Powercopy to instantiate multiple Hole features on a part like the above.

I want to thank all the folks who responded for your support.