loft with intersection curve

[Anonymous]

Hi everyone,

As I'm trying to get deeper knowledge of Inventor - could anyone please help me?

I'm trying to design a ring. It required some loft feature to be used. 

I've tried creating loft using Intersection Curve, but the lines didn't highlight - seems like this intersection curve wasn't affecting loft feature. Then I just used this Intersection Curve just to draw two sketches on both ends and only then Loft feature worked. 

What I don't get it - why this Intersection curve didn't work for the Loft? Then how I can use Intersection Curve effectively? When can I use it?

Many thanks in advance,

Milda

[DRoam]

The Loft tool will only work with 2D sketches. You can't loft between 3D sketches. So, you have a couple of options.

If the profiles you want to loft between are actually 2D profiles, just in the 3D sketch environment, then you can create a 2D sketch and project the profile onto the 2D sketch, and use the projected profile for the loft.

If, however, the profiles you want to loft between really are 3D profiles, then you'll need to use some surface modeling. Patch and Ruled Surface will be the most likely candidates. Followed by Stitch or Sculpt to make the resulting solid.

Hope this helps.

[johnsonshiue]

Hi! To add to Derek's comment, Loft does support 3D sketches. It is only available in Surface mode (Solid requires capping faces; it will work if the 3D sketch is a face loop).

In the Loft dialog, click on Surface. You will be able to select 3D sketches as sections.

Many thanks!

[Anonymous]

Hi Johnson,

I have tried Loft command in Surface mode. It only became active with 3d sketch 1, and sketch 23. After that if I tried adding anything else - Loft became inactive as if something is chosen wrong. That is why I understand why @DRoam said its not working on 3d sketches. And especially if you are studying Inventor on your own, these complications shows that either you are doing it wrong, or you think that it simply doesn't work this way...

Johnson, maybe you could try this loft feature on my drawing - maybe I need correction in which sequence I should choose sketches for Loft feature?

Thank you so much in advance,

Milda 

[johnsonshiue · Accepted solution]

Hi! I took a quick look at the files. I think I know what you are attempting to do. There are multiple ways to do it. When you use Loft, you want to keep things simple. Loft itself is a fairly powerful and versatile command. If you add too many constraints (geometry), you will make it very complicated leading to bad behaviors.

Like I suggested, I think you may want to consider using Surface modeling workflows. See attached part. You can use Stitch command to turn it back to a solid. Keep in mind that building a solid body does not mean you have to use Solid features. Surface features can help you manage intersection more easily.

Please take a look and see if you have additional questions.

Many thanks!

[Anonymous]

Hi Johnson,

I have followed your example using Boundary Patch and Stitch commands. 

I have done one example before using plane. In your example loft plane surface is following ring surface - how its supposed to be. 

In my previous example I was using loft feature under Solid command. I could add fillet of 0.25mm on the edges.

When I followed your example, I've done thicken command. It just allowed me to add 0.01 thickness. And I can't put any fillets on the edges. So I understand I should have used fillet command before adding thickness. (on this part should be added "diamonds" later on - so fillet command would be best at the very end - I think - I have attached the example of the ring I'm trying to recreate)

Also I wanted to make a cut through - and this part behaves differently than solid.

Could you please check the files I've attached with both examples. 

I appreciate your help,

Milda

[johnsonshiue]

Hi! I guess you are probably confused with multi-solid bodies. You have multiple solids. If you want to cut through, you will need to select the bodies. Or, you simply use Combine command to join them together.

One thing I would like to point out is about reverse-engineering. If you are trying to replicate somebody's design for learning purpose, it may be Ok (depending on the author's rights). If you are trying to do it for commercial purposes, I would ask you to stop unless you obtain copy right.

Many thanks!

[Anonymous]

Hi Johnson,

I'm registered with this website where various customers upload their jobs. Then candidates apply. I wasn't applying at the time because of the lack of knowledge. The image was available for all to download. So I'm learning at my own pace - no pay, no gain, just knowledge. 

Many thanks,

Milda

[Anonymous]

Johnson,

I've tried Combine command before - it just gives me a message "Could not combine bodies. The part must have at least 2 solid bodies". I understand that if the Loft would behave like a solid than I can apply fillet on the edges more easily. Could you please check how to make this part of the ring into solid?

And also I checked the Top view. The loft should have been more curvy looking from the top - right now its just straight lines. How can I make the lines look more like in Intersection Curve 3d Sketch  - I've attached the images. I want to make it to myself clear  for future references.

Thank you so much in advance,

Milda

[Anonymous]

Johnson,

I was able to sort out this curve when using Loft command adding guide rails of 3d sketch intersection curve - so that's sorted.

But I still need some help with converting this part of the ring into Solid.

Thanks,

Have a nice weekend,

Milda

[Anonymous]

Hi @johnsonshiue ,

I understand that I might use Fillet feature on the part before the Thicken/ Offset command. But still I'm concerned about that part which is sticking out - I've attached the files for comparison.

Could you please help me out as I lack of ideas. 

Thanks a lot in advance,

Milda

[johnsonshiue]

Hi! It looks like the solid extrusion yields better result for you. Then you should stick to it. Surface modeling has its own limitation too. It would not solve every design challenge. The reason I brought up surface modeling is that often time our users seem to believe solids can only be done via solid features. Inventor does not have extensive surface modeling tools but it does have good ability to do surface modeling.

Surface modeling and solid modelings should be used whenever it makes sense and whenever it makes the job easier. It should not be exclusive.

Many thanks!

[Anonymous]

Hi Johnson,

Thank you for coming back to me. 

I just wanted to find out the limits of surface tools - maybe I was missing out on something. 

So after adding fillets before Thicken feature and few more closing walls - your example, while using surface modelling tools, looks better. Its much more precise, you can get the loft curved, not straight. Just attached couple of images for comparison.

Thank you so much for your help,

Milda