Curve driven pattern problem

[TobiasZetterberg2067]

Hi, I'm modelling a helical shaped finned tube heater and ran into problem with "curve driven pattern".

I have a tube that is sweept along a helix and a finn that is also sweept along another helix. When I try to pattern the fin along the helical tube it goes all wrong. Inventor only suggests the fin to be patterned in a straight line perpendicular to the helix curve (see attached picture). I use the procedure with "Rectangular pattern" and use the helical curve in 3d-sketch as "direction 1", I also set the orientation of feature to "direction1". I tried to do this with features that was extruded or revolved and it works just fine but there seems to be a problem when the patterned feature is sweept. I also attached the .ipt if that can be to any help. /BR Tobias

[CCarreiras]

Hi!

Select where it beggins

[TobiasZetterberg2067]

Hi again and thanks for your reply!

That works for distributing the feature along helix but the orientation never aligns to the helix. If I use "orientation-identical" it don't rotates at all (as it should be) and if I use "orientation-direction1" it suggests to turn it 90 degrees but won't perform the operation (create rectangular pattern failed). 

[CStilesCARE · Accepted solution]

Not sure why it makes a difference, but instead of selecting the center curve line, select the one running along the inside of the tube. Seems to make it align better on my attempt.

[CCarreiras · Accepted solution]

I believe this is a bug for this particular part.
I guess is due the plane for the washer sweep is "parallel" to the helical curve, so the pattern direction is also parallel... how knows...

Anyway...

Since you probably will need a final assembly, the pattern will work in the assembly if using the Construction point pattern existent in the tube part... it's another option to consider.

[TobiasZetterberg2067]

Hi again! Both tips worked great. Thanks or all your help!

/BR Tobias

[TobiasZetterberg2067]

And the result...

[CCarreiras]

Nice!!

Put it here:

https://forums.autodesk.com/t5/inventor-forum/community-pictures-march-2023/m-p/11789852/highlight/f...

Also, if you have time, send the part to development to analysis and correct the issue.

[CStilesCARE]

Hey hey, that render looks nice! Would take my computer days to create, I'm sure lol.

Glad we were able to help!

[johnsonshiue]

Hi! Another approach without using the patterning is to create a Twist Sweep (see attached image) as a surface body. Then thicken it to a solid body.

Many thanks!