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

[gmwi]

I have found that the closer the sketch is to the curved surface before projection, it works a lot better. Just make your 2d sketch planes in reference to your curve surface.The program is calculating the points based on start distance to finish point. Think of it as setting a bottle on a table in front of you and place a i.e "label" on surface. Fits pretty well, but move the bottle to the other side of the table and then place the "label", not the same prospective.

[cadman777]

Find attached one of my versions of it from IV2010.

The complexity depends on the blade profiles, which drive everything but their length.

When you change the BladeTwist angle dimension the first 3d sketch breaks, so you have to go into it and move the lowest lines back up with 3dMove&Rotate. I always have had this problem w/3d sketches. Maybe someone in here can explain how to prevent the sketch from flipping like that? But otherwise, things should automatically adjust if you change the sizes of features, within reason that is.

I made the blades .003" press-fit (that's .015 OAL interference for each blade). You can see that in the drawing.

Also note that I only approximated your blades b/c they were impossible to measure accurately.

[engisu]

Hello gmwi,

I've attached a part that is a little more complex of a profile. I have it setup with the planes closer to surface like you had said. I have this exact part with the plane far away and still am dealing with the same issue. I'm able to create the loft, but still have an issue with creating a loft that doesn't require merging tangent faces. Both sketches are equal with the same amount of arcs so everything should loft fine, but I'm still having issues.

Anyone have a workaround to not have to merge tangent faces? This part would be more of what I'm running into. The other example might have been simple enough that it didn't effect the outcome of the loft.

Thanks

[gmwi]

Well I'm limited on helping at this point because Inventor will not save the history tree. I'm running '21 and can open your model but it's an import with history tree. You could export the sketches as dwg/dxf and then I can have ago with it.

[engisu]

Attached is .DXF files for the ID and OD profile. The ID gets projected to a 5" Ring ID and the OD gets projected to a 7.8" Ring OD. The upper most part of each fin has a radiused top, the center of that radius is centered with the part.

Let me know if these files work or not.

Thanks

[gmwi]

I've got a process for you. Don't use 2,  3d sketches. You can use 2d to 3d OR 2d to 2d. If you use 3d to 2d , choose the direction correctly because the program gets fussy about it. When you go from 3d to 2d it fails on the array feature. Going from 2d to 3d direction allows it to calculate as it likes and will array. I've included both versions and the comparison between the two different approaches to show the differences in surface creation. If you get into more complex shapes , you'll need to include guide rails or if REALLY involved then "surfaces" are the answer.

   

[engisu]

Thanks for the reply. So there isn't a way to use 3d to 3d without merging the faces? I mainly ask this as I can get a better representation of the fin this way than trying to extrapolate to where the think the fin should end in space.

When using the 2d sketch in the problem it will shift the surface off from where it should be. It seems to generate surfaces easier, but solid works best for the CAM program.

Seems like if I can't go 3d to 3d that my issue has been as solved as it can get unless they make a change to the software.

Thanks for your help

[gmwi · Accepted solution]

Ok if you want to use 3d to 3d loft. Then add guide rails and then loft as a surface. You have to "cap" the ends before it will let you stitch to make a solid. Then array the solid feature as needed. Side note, you can still use surfaces for CAM options.

    

[engisu]

That's just what I've been looking for! Works real slick for how I currently do the process.

Thanks again for everyone's input!

[cadman777]

That's how the model I posted is made.

Check it out @ # 15 of 30 above...