How Do I Perform A (Relatively Simple) Loft

[Anonymous]

Hello Folks,

Disclaimer: Longtime SolidWorks user.

I am desperately trying to create a lofted feature. This feature is rather simple in comparison to some things I've done quite easily in the past using SolidWorks.

There's a closed profile at the top and another at the bottom. When I invoke the Loft command, I select the top and bottom profiles and Inventor previews a solid body that represents a simple, striaght projection. The problem is when I select a Rail (or any combination of Rails), the solid preview disappears and I get error messages of varying vague content.

I have yet to select the two profiles and a Rail and have Inventor produce a solid Loft. I have tried several variations of geometry and methods of invoking the Loft, including simpifying the process.

Here comes the part where I appear to prompt abuse from others: This is something that is so painfully simple in SolidWorks that, using SolidWorks, its easy to create Lofted features that are not what I want the end result to be. But, because SolidWorks actually returns lofted geometry, right or wrong - by selecting multiple profiles then one or more paths - it's easy achieve what I want by process of elimination. By playing.

This is something that is important for me to learn.

The part I've attached is an attempt at creating half the part, then mirroring the Loft to create the desired part.

Mel

[TheCADWhisperer]

You should indicate what version of Inventor you are using (files are not backward compatible).

I noticed many unconstrained sketches (missing dimensions and Tangent constraints).

At least one of your Rails (Guide Curves) is not attached to a profile.

Can you download a 30-day trial of 2017 to make communication easier?

Guide Curves must have tangencies - I suspect this is also true in SolidWorks.  I will give it a check when I have a chance.

[mcgyvr]

https://knowledge.autodesk.com/support/inventor-products/troubleshooting/caas/sfdcarticles/sfdcartic...

[jtylerbc]

While I would agree in general that many of the error messages in Inventor are vague to the point of uselessness, the ones received for this part are not, and actually do tell you exactly what is wrong.  They actually are telling you exactly what is wrong.

You have a variety of issues in this part, some of which occur in multiple locations.

1. Almost everything (including the two profile sketches) is underconstrained.  You are missing many geometric constraints as well as actual dimensions.  This is definitely the root cause of some of your guide rail problems, and may be involved in others as well.
2. As @TheCADWhisperer mentioned, one of your guide rails (Front-Right corner) doesn't touch the upper profile.  The error message received when using this guide rail specifically mentions that as being the problem.
3. At least two of your guide rails (Left side) give errors about not being "Smooth."  This is caused by missing tangent constraints in Sketch3.  Guide rails need to be tangent-continuous, which is what the error message means by "Smooth".
4. One of your guide rails does work as-is (Right-Back corner).  It is continuous (no way to mess that up in this case, because it is a single line), and it properly intersects with both profile sketches.

[Anonymous]

As so many have mentioned before, the majority of the issues are the underconstrained sketches and the fact that some of the guide rails are not intersecting the loft profile (as the error messages say). I went and quickly fix SOME (not all) of the issues and was able to successfully loft the profile with the guide rails. See attached. 

[Anonymous]

Hello Folks,

I am apply changes as you folks have suggested. I am getting closer as I am actually producing Lofts.

It is not only difficult to apply constraints, it is difficult to determine whether-or-not a constraint has been applied or whether-or-not a constraint already exists.

As I've said before: constraints are easier to apply, observe and manage in SolidWorks.

I do appreciate your help and, if you like, I can post the finished part.

Thank you,

Mel

[Anonymous]

Use F8 to turn on the visibility of constraints, and F9 to hide them. Also, when you click on a line, arc, etc. you will see the constraints that are applied (if any).

It sounds like the majority of your issues are coming from not being familiar with the fundamentals of Inventor, and trying to do too much too fast. It might be good to go through some of the early tutorials (sketching especially) and get more familiar with the basics. 

[Curtis_Waguespack]

Hi melvin.burk,

I noticed this in your profile:

"At my current place of employment, fully constrained and dimensioned sketches are frowned upon as constraining and dimensioning are considered a waste of time. I want to learn - even master - Inventor but also want to remain employed. So please, bear with me."

I am in no way meaning to cast stones, but I feel it is important to mention that not fully constraining and dimensioning sketches will preclude you from learning and mastering Inventor, as it will be a very frustrating journey

Maybe Fusion would be better fit for your workplace? I think it allows a bit more freedom with some of this, but someone can correct me if I'm wrong.

http://www.autodesk.com/products/fusion-360/overview?src=OMSE&mktvar002=638405&mkwid=sH3Auec2W|pcrid...

If you must continue to use Inventor, would it be possible for you to share a bit more about your design inputs, so that we can understand how you arrive at the size and shape of your sketch profiles. I see a few things in the example part that puzzle me. But I'm sure there is a very good reason for them. Understanding some of this will likely lead someone to be able to better help you simplify your process quite a bit.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Hello Curtis,

I agree, not constraining or dimensioning sketches will hinder the development of my Inventor skills. 

I am currently working a contract position. The only influence I have is to do the best work I can with the tools available to me. We currently have Inventor 2013 and are not likely to buy anything else soon.

I've updated my forum profile to explain my Inventor process at my current employer.

We basically replicate old, heavy and (often) damaged pieces of decorative clay. 

My background is the documentation of repeatably manufacturable parts and am not used to the less-than-optimal engineering practices used here.

Mel

[Curtis_Waguespack]

Hi melvin.burk,

If I can find time, I'll make a screen cast of that part, that will demonstrate one method to do this with far less sketching required.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Hello Curtis,

That would be appreciated. I'm getting pretty close but cannot get the Loft to include the long, curvy line about the top of the part as a Rail.

Again, I agree. I have to create more sketches using Inventor than I do with SolidWorks.

One thing that bothers me about Inventor compared to SolidWorks is Inventors inability to use existing sketch or reference geometry as objects to be used in subsequent sketches.

For example: in SolidWorks I could create a new sketch then offset geometry from a previous sketch without having to "project" that geometry into the new sketch first then having to deem the initially offset geometry as "construction" geometry. The same thing with using planes or points: in Solidworks I could create a new sketch then associate new sketch geometry from existing planes or points as opposed to "projecting" that plane or point first then having to deem the initially associated geometry as "construction" geometry.

Thank you,

Mel

[Curtis_Waguespack · Accepted solution]

 Hi melvin.burk,

Okay here's one approach (slightly simplified for time sake). Of course I might have started with the profiles where as you might need to start with the base shape, depending upon what you have as design inputs, but this demonstrates the use of simple sketches and multiple bodies for this type of thing.

Use the Full Screen arrow to view full size.

And sorry for going to fast.   Just use the pause and rewind buttons as needed. And post back if you have questions.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Part 1

Part 2

[Anonymous]

Hello Curtis,

That is interesting. Using two extruded entities (disjointed bodies, and their position in space) proves the integrity of each profile and makes it easier to define "Rails" and to select their profiles as Loft entities.

Am I interpreting your method correctly?

Mel 

[Curtis_Waguespack]

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@Anonymous wrote:

Am I interpreting your method correctly?

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Hi melvin.burk,

Yep, that's basically it.

I prefer solid geometry over wireframes and sketches whenever possible. And I prefer simple base features, an simple secondary features to create more complex shapes always. I used to teach Inventor to professionals of all skill levels and found that working in 3D and keeping sketches simple is simply easier for all of us.

Having said that, many of us were taught to sketch out 2D profiles for lofts, etc, and so we do it that way out of habit. So many experienced people would likely do it that way still. And there's nothing wrong with that at all. I've just learned (the hard way) that keeping the 2D simple and working with 3D solids as much as possible, just seems to work better, and makes edits easier.

I suspect for the type of work you're currently doing, you could use the multi-body approach to create all of the inter-related parts in one "layout" part file, and then use the Make Components tool to write them all out as individual files. That would allow you to more easily reuse the profiles of part1, to establish the mating face for part2, and reuse the profile of part2 for part3, and so on. But I might be assuming too much about your overall workflow. In any case post back in the future if you see those opportunities.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Hello Curtis,

Great! I'm employing this method now and expect a better part with a simpler feature tree.

I wish you were right about developing our models with the intention of them being related. Unfortunately, most of our work is spot replacement: select disparate pieces of a building where replacement is based on condition.

I can't wait to develop a large, cohesive set of models.

Your input will go a long way in making Inventor a relevant tool around here.

Mel

[Anonymous]

Hello Curtis,

I'm not experiencing the same phenomenon when you "Delete Face" in your video. I can't make those initial "walls" go away like you did.

The location of that command appears in the "Surface" tab of Inventor 2013. You appear to be invoking the "Delete Face" command through the "Modify" tab.

I'm not sure if my experience is different because I'm running Inventor 2013 or because I can barely see what's going on while you're working.

Mel

[Curtis_Waguespack]

Hi melvin.burk,

1. I probably just went too fast through that part of the video, but be sure you've expanded the video to full screen as well (see button in lower right of the video player).
2. The Delete Face tool has evolved and didn't get renamed or updated well, so it's not real intutive. It's really a Delete Object tool now.
3. Indeed they did move that tool from the Surface panel to the Modify panel in Inventor 2015.

In any case you want to choose the  Select lump button as shown:

I checked the 2013 help files just to make sure that button is there, and that I wasn't misleading you, and was relieved to see that it is there (I think it was added in Inventor 2010 when mutli-body solids were introduced):

http://help.autodesk.com/view/INVNTOR/2013/ENU/?caas=caas/vhelp/help-dev-autodesk-com/v/Inventor/enu...

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[TheCADWhisperer]

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@Curtis_Waguespack wrote:

Hi melvin.burk, 

In any case you want to choose the  Select lump button as shown:

I checked the 2013 help files just to make sure that button is there, and that I wasn't misleading you, and was relieved to see that it is there (I think it was added in Inventor 2010

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FYI - This tool has been in there as far back as I can remember.  Checking old documents - I was writing about using it in 2006.

I found a reference from before I started with Inventor (I assume it had the Lump or Void options in addition to Heal back then) https://forums.autodesk.com/t5/inventor-forum/love-quot-delete-face-quot/m-p/554024/highlight/true#M...

[Curtis_Waguespack]

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@TheCADWhisperer wrote:

FYI - This tool has been in there as far back as I can remember.  Checking old documents - I was writing about using it in 2006.

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Hi TheCADWhisperer,

The Delete Lump button has been around that long, or the Delete Face tool?

The Delete Face tool has been around for as long as I can recall, but I was thinking the Delete Lump button was added more recently, but I might not be remembering correctly.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[TheCADWhisperer]

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@Curtis_Waguespack wrote:

 

The Delete Face tool has been around for as long as I can recall, but I was thinking the Delete Lump button was added more recently, but I might not be remembering correctly.

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Image from a 2006 tutorial that I wrote -