Circular Pattern Failure on Loft

[engisu]

Hello,

I'm looking to get help with properly setting up my part so I have a no fail process to produce a complete modeled part. I'm creating a fin that is connected to an inner and outer ring. I have a normal sketch and using a 3d sketch to project to a surface. This is done for both the inner and outer part of the fin. I then use another sketch to make rails to better define the surface it creates.

I've had issues with this generating sometime, but the attached part generates well and then has issues with the circular pattern. In the past I've had to merge tangent faces to get it to even generate the loft, but would like a problem free solution if there is one to do this process.

Looking for any help that someone may have to solve this or if I'm approaching this wrong.

Thanks

[cadman777]

Are they all separate parts, or is it a casting, or something else?

[engisu]

Hello Cadman,

The part I'm currently working on is a cast part. Looking to make it a one
piece. This file is just a generic representation to get the point across
without giving out my model. In our other parts the outside ring is one
piece and the rest another piece.

Thanks

[cadman777]

OK, so do you  weld the ring to the rest of the casting?
Is any pre-weld machining done on any of the parts?

[engisu]

The ring is a shrink fit. May I ask why these questions are applicable to
what I'm looking to do?

Without scanning OEM piece and creating it that way, I can create these
sketches and project them. This way if I want to modify the profile its
much simpler. Just looking for a guaranteed approach to creating this fin
and being able to circular pattern the fin.

Thanks

[cadman777]

Why the questions?
I have an older version of Inventor so can't see your 3d model.
I have to look at it in the Autodesk online viewer and guess at what the dimensions are.

Another answer:

When I make a part like this, I take into consideration how it's fabricated. So if the whole thing was a casting, I'd make it differently than if the outer ring (rim) is separate from the hub+fins, or if all parts are separate and fitted/welded together. Since this consists of 2 separate parts, it is an assembly. But it can be effectively made as a MultiBody part.

This shouldn't be too difficult to do.

I'll give it a go tomorrow.

One assumption is the fins are curved in both directions.

[engisu]

Oh sorry about that, I can save it back as an older version if needed
tomorrow.

Typically when I create parts like this the outside ring is separate. I
usually would only use the outside for a surface to loft towards if I'm
trying to replicate a factory part and make it billet. The ring would then
be removed from the part. Usually for machining parts like this swarfing is
the main toolpath but with a one piece part makes machining quite a bit
more difficult. I would like a way to use an inside and outside diameter
ring as this is something that can be physically measured and recreated
into a model. Unless you think I may be approaching this incorrectly?

Thanks for your help with this, I do appreciate it!

[cadman777]

Sounds good.

If you post a STEP file, I could read that.

Incidentally, I'm using Inventor 2010.

[JDMather]

---

@engisu wrote:
Just looking for a guaranteed approach to creating this fin
and being able to circular pattern the fin.

---

Pattern of Body is more robust than pattern of Feature.

See Attached.

[JDMather]

@cadman777 

You should probably add this information to a Macro or to your signature.

Example:  I am running Inventor 2010 and cannot open newer files.  Can you please attach images and STEP version of the geometry in question?  Thank you.

[cadman777]

Great idea. Thanx! Let me give it a try.

Last time I tried editing my profile it didn't work, so I just abandoned that idea.

But that was many moons ago.

Back then I just figured it was another Autodesk SNAFU that I had to WORK AROUND, so I abandoned the idea, like I have with many of their half-baked software functions.

[engisu]

Hello JD Mather,

I've done that before, the only thing there is it also repatterns the inner and outer parts that aren't the fin. This problem usually arises when I have slots and other geometry that is part of the part model in the inside, so depending on the fin number all of this is usually depleted by the patterning of the fin.

So that being said is this something that is best done after a revolve and then do any inside geometry work in the middle of the part? Or is there a workaround to just circular pattern the fin? My main reason to have the work around is if I a base part and want to create new fin geometry it may make it a little tougher, but this is seeming to be the way to work around this. I can add some example of inner geometry if you need to explain this further.

My main reason for creating the post is sometimes when I use the project a sketch and then try to loft the 3D Sketch even though everything looks good it fails to build the loft. Not sure if all points and lines included need to be projected or if I missing something?

Cadman, I've attached the STP file of the part. Hopefully this will help make things a little clearer.

Thanks

[cadman777]

Thanx for the STEP file!

[nedeljko.sovljanski]

Hi @engisu 

Yes there was some issues with loft, but I have success with loft as surface, patch top, bottom and Sculpt. 

[engisu]

Hello nedeljko.sovljanski

Looking to stay with a solid at this time if possible. I noticed as well when trying to loft a surface this also creates issues when trying to circular pattern as it wouldn't generate due to not producing a meaningful result.

Thanks

[nedeljko.sovljanski]

Hi @engisu I am still on this thread and it seems only solution, if you want to stay on solids, is @JDMather "Pattern of Body is more robust than pattern of Feature." Here is way. If you have non planar sketch (3dSketch) you can create loft only with join operation (it can not create new solid). So if you try to make some pattern and choose only feature, your loft has no top and bottom surface. Your loft use common (inner and outer) surfaces. Because of that you need to include them in pattern, and that means use body instead of feature for pattern type.

---

[gmwi]

Try this. You can rotate the features but you do need to structure your builds. The program likes to take everything in previous history back to the start of a solid. So if you make a feature as a new solid or multi-solid then it starts at that point.  Either way, select the features you want to polar array.

 

[engisu]

Hello All,

Seems like the circular pattern issue will have a work around. Does anyone have input on the best way to take a planar sketch that can be measured from an existing part then projected to a surface? Mainly looking for this answer to see what issue with the method I'm not seeing. I've had it where the green rendering for the loft looks perfect, but then it says it failed to produce a meaningful result.

Thanks

[gmwi]

You can project the 2d sketch onto a 3d surface. You need to keep in mind about the distance you place the projected sketch to the surface.

 

[engisu]

When projecting a sketch to a surface. If the sketch plane is 1" away from the closest point of the surface and then another example is 0.5" away this will make a difference? I'm using the project to surface along vector. Was assuming with the software it was moving straight with the plane to the surface or does the distance cause issues sometimes with being able to hold a certain level of accuracy where it can adequately project the sketch?

Thanks