Pattern to twist with a geometry

[Garbean]

Dear PTC-Community,

I have been stuck with a design challenge and come to you as my last resort of maybe finding a smarter solution to my problem. I'm using creo 9.0.3.0.

I'm trying to put 0.6mm holes which are 1.2mm apart from each other trough a body that is "twisted" in space. (It is part of a fan blade)

I want the holes to enter the part on one surface and exit on the opposing one. They need to follow the geometry, but the entry and exit surfaces are not parallel to one another.

My best approach so far was to make a row of profiles on a plane perpendicular to the direction in one corner of the part and use the "Pattern" - "Curve" function, selecting one of the edges as the reference curve. I also choose the option "follow the surfaces", and select the entry and exit surface. I hope the following screenshots make my process more easy to follow. It's difficult to explain, what I want to archieve.

Profiles on the top, following the top left edge of the part.The pattern following the profiles.

This gives me the following result, which seems to generally do what I want to archieve. In the top part everything is working very well, but towards the bottom of the part, the profiles seem to slip off the desired trajectory. I need the holes in the bottom part to be like the ones in the top part, entering and exiting the front and back surface. Video of result:

The holes will be archieved by subtracting the two bodys, after I manage to align the profiles properly.

Any hints as to how I could solve this issue, or alternative approaches will be highly appreciated!

Thank you for your time reading,

All the best

Garbean

[Garbean]

Adding some screenshots of the result, as the video does not seem to work just yet.
Result front view. (Looks kind of good and like the thing I'm trying to archieve)Result back view (See how the Pattern drifts of the geometry in the lower quarter of the part?)

The front view (left) looks kind of like the thing I'm trying to archieve. The back view (right) shows how the pattern deviates from what I want in the lower section of the part.

[tbraxton · Accepted solution]

This is a sample of a pattern of cylinders extruded normal to the center point of the cylinder on the reference surface (purple quilt). Is this representative of the general problem you are attempting to deal with? I am assuming that you can generate a neutral axis surface between the entry and exit surfaces that the holes penetrate. Using this approach, you can pattern the holes such that they would lie within the bounds of your part solid faces assuming it is possible using straight holes.

[Garbean]

Dear tbraxton,

Wow, I'm impressed! Thank you so much for your quick reply. That looks like a really clean and smart solution.

How do I go about creating that neutral axis surface and which pattern options did you use in your example?

I can't wait to try this out tomorrow..

Garbean

[tbraxton]

Here is a Creo 7 model that will demonstrate the pattern and grouping used in my example. 

Without the geometry it is hard to determine how to approximate a neutral axis surface. I created the neutral axis surface first and then thickened it for expediency. If your proximal and distal faces are not offset, then you will need to make some approximation of the reference surface.

I think I would cut the faces after the holes are through the body if possible so you can exploit some geometry of the body you are putting holes through.

[Garbean]

Thank you tbraxton for providing a working example. I did as you suggested and it is the perfect solution to my problem. Could not be happier, thank you for ending two weeks of fiddeling around not getting statisfying results..Learned that I can make patterns of groups, which will be helpful in many cases.

Screenshot of the result:

[MartinHanak]

Hi,

FYI if you upload video as attachment then it will be available immediately.