topic Re: Ergonomics: Trying to overcome Loft limitations ...and limits. in Inventor Forum

Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Fri, 13 Apr 2018 10:38:16 GMT

Usually the ergonomic shapes (handles, grips etc.) but not only (think aerodynamics, product fasion etc.) are made via Loft and/or Free-form. We can see this trend everywhere around us in almost any electronic gadget from kettles to drones etc.

In our discussion, one of the main limitations of the Loft engine is its ...limits. Loft starts from a plane (sketch), „goes” via other planes (sketches) and finishes to another plane, making impossible to „attach” the lofted feature to another non-planar face/feature. See the red-marked gap in the image below:

Loft to non-planarWe can „fake” this attachment by using an extrusion from the latest loft plane like in the image below, however the lofted shape changes as you can see in the following image:

Loft to Extrude to non-planar

What we really need IMHO is an extension to the Loft command which will take the first/last sketch, project it to a (non-)planar surface and start/finish the Loft from/to said projection.

I am thinking to post this as an idea. ...but perhaps I am missing something? Any other thoughts?

PS: for your convenience, you have the above ipt files attached.

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Fri, 13 Apr 2018 13:59:14 GMT

Just wondering, would a Face Fillet serve a purpose in this situation?

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Fri, 13 Apr 2018 15:39:29 GMT

No, because usually there are two solid bodies (eg. the handle and the body) which we want to join and Face Fillet works only on the same solid. It is a shame, I know. Isosurfaces must work „anywhere”. POVRay has these from ...I don't know. 20-30 years ago?

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

PaulMunford — Fri, 13 Apr 2018 16:59:13 GMT

To clarify - would you like a 'Loft to [surface]' option? Like 'extrude to'?

As a workaround, you could try 'replace face', or intersect the loft plane with the first body and use a Boolean to clean up.

Does that help?

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Fri, 13 Apr 2018 17:48:13 GMT

@PaulMunfordwrote:
To clarify - would you like a 'Loft to [surface]' option? Like 'extrude to'?

Yep, this is the idea.

@PaulMunfordwrote:

As a workaround, you could try 'replace face', or intersect the loft plane with the first body and use a Boolean to clean up.

Does that help?

Well, I think so, but as you realize is too complicated. Besides that it is a kludge - it needs additional „scaffolding” which can be (very) difficult to create / manage / fit.

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

johnsonshiue — Fri, 13 Apr 2018 20:51:54 GMT

Hi John,

I would argue the issue is more about solid geometry creation than Loft. This case would be much easier done via surfaces and then sculpt or stitch them into a solid.

Solid features offer less control on intersection and termination. It is because every solid feature has to ensure the resultant body be water-tight. This requirement limits the flexibility of intersection and end treatment.

Many thanks!

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Sat, 14 Apr 2018 06:20:50 GMT

Hi Johnson,

@johnsonshiuewrote:
Hi John,

I would argue the issue is more about solid geometry creation than Loft. This case would be much easier done via surfaces and then sculpt or stitch them into a solid.

🙂 I certainly understand what you're saying, however surfaces / free-forms cannot give us an exact profile, neither the parametric paradigm which is the main selling point of this program. If we'll have profile constrains and/or full 3D parametric engine applied to surface(s) the things change. We have some steps in that direction (3D annotations and 3D dimensions / constraints in 3D sketches) but we aren't there yet.

@johnsonshiuewrote:
Hi John,

Solid features offer less control on intersection and termination. It is because every solid feature has to ensure the resultant body be water-tight. This requirement limits the flexibility of intersection and end treatment.

Hum, ...but here water-tight is a feature, no? We want to have a water-tight body since the final result will be manufactured via an additive/substractive method isn't it?

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

johnsonshiue — Sat, 14 Apr 2018 15:18:22 GMT

Hi John,

We are talking about the same thing. I think you might have misunderstood what I meant. I am not saying we should create loose geometry or use Freeform for everything. It does not make sense. Freeform is good for organic shape but it is very difficult to achieve precision. My proposal is to create the Loft using Surface Loft instead of Solid Loft. You can easily extend surfaces to intersect with bodies while you would have hard time doing the same to a solid body.

Certainly, the objective is always to get a water-tight solid body in the end. However, you don't need to limit yourself to solid features. You can use surface features (as well as Freeform) to create a water-tight solid body.

Many thanks!

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Mon, 16 Apr 2018 10:12:48 GMT

Thanks That worked!

Unrelated to main topic but related to our discussion:

Why I cannot change the Loft from Solid to Surface? (this applies to other commands also)

You know, have a Solid Loft, RMB, Edit Feature and in Output group box to click on the Surface button?

It is a fairly complex command and it would be very nice to have this feature, even if it wold be accomplished by demolishing everything internally and rebuilding from scratch. It saves us from entering the same parameters again.

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

SBix26 — Mon, 16 Apr 2018 13:44:53 GMT

You can turn a solid to surfaces very easily by deleting a face (Delete Face tool). Happens accidentally whenever I forget to check the Heal box...

Sam B
Inventor Pro 2019.0.0 | Windows 7 SP1
LinkedIn

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

johnsonshiue — Mon, 16 Apr 2018 15:56:37 GMT

Hi John,

I wish Inventor could be much easier to use. There is room for improvement in every corner of Inventor. The main reason why a solid extrusion cannot be converted to a surface extrusion is that such conversion will only work if there is no dependent features. When there are dependent features to the extrusion, allowing such conversion will invalidate most dependent features.

Technically, a body is a body. It does not matter it is solid or surface. This is why hybrid modeling technique (solid and surface) is a powerful tool in mechanical design.

Many thanks!

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Tue, 17 Apr 2018 10:46:19 GMT

@johnsonshiuewrote:
Hi John,

I wish Inventor could be much easier to use. There is room for improvement in every corner of Inventor. The main reason why a solid extrusion cannot be converted to a surface extrusion is that such conversion will only work if there is no dependent features. When there are dependent features to the extrusion, allowing such conversion will invalidate most dependent features.

Hi Johnson,

Hum.... yep. In my attached file there aren't dependent features AFAIS - and *I* am the user. 🙂 (IOW, as you know, what the user sez matters most).

Besides that, updating with dependent features is already solved for dimensions. In fact this is the main selling point of the program.

Otherwise we have a ton of options ranging from Rhino, 3DsMAX etc. till Blender & co.

And more: Updating with dependent features is much easier in this case, compared for example with Data Definition Language (DDL) from SQL databases because DDL has to preserve the data which there is the most important asset whereas here „the data” is exactly the DDL (the model) hence, if I change an option the engine can use as a last resort the blind brute-force regeneration of all the dependent features downstream (of course, optimizations can be employed), thing which already happens when we change the topology of the sketches etc.

So why when we can change a topology (which can easily blow up things downstream especially when we trim/delete lines etc.) and we cannot change an option in a command?

Now we are in the middle: iLogic is a non-visual way to describe the 3D space but we can change „anything” inside (it is a matter of editing a text file) while in Browser/Model which is a visual way to keep a list of commands (much easier to use) we aren't allowed to do the very same thing.

Technically, a body is a body. It does not matter it is solid or surface. This is why hybrid modeling technique (solid and surface) is a powerful tool in mechanical design.
Many thanks!

Yep. So we are settled, isn't it? Hybrid modelling will be in next release ...how many weeks ...ahem... hours from now? 🙂

Just joking. 🙂

Seriously tough, IMHO we must unify from an user perspective some things the most important now are being for me the 3D parametric engine (dimensions / constraints on free-forms etc.) and editing engine.

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

johnsonshiue — Tue, 17 Apr 2018 19:11:25 GMT

Hi John,

I think you might have misunderstood my comment. It is true that Inventor does not allow users to convert an existing solid extrusion to a surface extrusion. What I was trying to say is that if we did allow it, it would only work when the body does not have any dependent feature. It would have been very restrictive, which diminish the value of such workflow.

Regarding keeping associativity, Inventor is structured in a way that a solid body is a different body type than a surface body. Although one can argue that, it does not have to be this way (like I said earlier, a body is a body). However, there are certain operations only generating certain body type. Not every command is like Extrude which can create a solid body and also a surface body. Mixing the two can lead to more confusion.

Hybrid modeling approach can be done in Inventor for years. It is just that some users assume creating a water-tight solid can only be done via solid features. It is a common misperception. Certainly, it would be great if Inventor had more surface modeling ability.

Many thanks!

Re: Ergonomics: Trying to overcome Loft limitations ...and limits.

Anonymous — Wed, 18 Apr 2018 11:01:19 GMT

Hi Johnson,

Thanks for the reply! Sorry, perhaps I wasn't very clear.

Let's try another approach.

You say:

@johnsonshiuewrote:
Hi John,
I think you might have misunderstood my comment. It is true that Inventor does not allow users to convert an existing solid extrusion to a surface extrusion. What I was trying to say is that if we did allow it, it would only work when the body does not have any dependent feature. It would have been very restrictive, which diminish the value of such workflow.

I say that this problem - „editing prohibited because dependent features exist” - is already solved in other worlds / industries / programs etc.

For example in SQL database world we have very tight references between the objects. For example, you can see below the dependent objects of a small table (the 1st one which I've found):

So, in simple therms, in order to change the definition of the „object” you see, the database server must update all the „dependent features” (the „Referenced by” column) which rely on the „object”.

In our case, because:

- by changing from solid to surface (or vice-versa) the topology is not changed (or, at least, not drastically)

- the „dependent features” do not have data outside of the model.

...Allowing this change is easy to do by re-applying all the „dependent features” on the said „object”.

This is the way in which works in database world. The very same way is used in the state-of-the art Raw photo editing. Because Raws are regarded as „valuable asset”, all the editing is NON-distructive and all the edits are saved in a separate file (called „sidecar” or XMP file) in an XML-like file, resembling very much our Model. The user doesn't see this file, he only sees his edits AND the final image which is the result of these edits applied in order. See them there:

Non-destructive editing

If the user changes one of these edits by dragging the sliders on the right, the program (Adobe Camera Raw in this case) re-applies „quickly, quickly” all the downstream edits to the image in order to update the final result. In the same way a program can regenerate a 3D model if the user changes a feature which has dependent features. If the program cannot do this will throw the classical error with „Accept,Edit,Cancel”.

Why we can change the Extrusion depth and/or Join/Cut/Intersect(!! which can change a lot the topology) but not the Output type (which keeps the topology more or less the same)?