practice - impeller housing - SHELL

[pb_max]

I cannot get the shell feature to work on the extended plenum.  It fails no matter what settings i put in AND Creo locks up for a good long while after I select the rounds to exclude.  The excercise asked for the rounds to be added first, so I assume it was focing that issue.  I also initially left the main housing unshelled, but when this issue arose,  I shelled it seperately in insert mode and it worked FINE.  I tried both single surface removal and both ends like I want.  I am including the model with the failed feature as reference.  Any help is appreciated.

[JohnWalker-TCD]

Hi,

Thank you for engaging with the practice at the end of the fundamental courses. I took a quick look at your model and noticed a couple things:

• You have two shell features, and it is the second shell feature that is currently failing. Remove the second shell feature. You can complete this model with only one shell feature.
• Move your "Shell 1" feature further down in your Model Tree and edit which surfaces are removed.

However, on your issue about creating the round prior to the shell, this is a result of your internal sketch for "Revolve 1" not matching the drawing. More specifically, the location is incorrect and needs updated. Once it is updated, you will notice the plenum sits further back on the housing which would result in your current "Round 1" extending further back than it does now (see the screenshot of the model in blue for reference).

Doing the above, I was to modify your design to obtain your intended outcome.  Give this a try!

John

[pb_max]

Hi John,

The top-most Shell was the one I mentioned adding in insert mode to get ANYWHERE at all...the original Shell (now shell 2) just fails whether I select 1 surface or both (the end of the scoop thing and the large round face with bolt holes).

I am not sure I understand about the Rounds...they had no issue themselves and went on just fine, but trying to exclude them from the Shell cause the system to lag, I just thought they could be the reason the Shell is failing?  I tried the Shell both WITH them excluded and WITHOUT.  Below when I moved the sketch, they still acted this way, although to a lesser degree.

"internal sketch for "Revolve 1" not matching the drawing. More specifically, the location is incorrect and needs updated."...ok, hmmm.  I moved the sketch, and the rounds are still valid, but Creo still doesn't allow the Shell, with any combination of selections...single surface, double surface, exclusions, no exclusions.  All fail.  To be clear, I removed the top Shell and moved the sketch as you suggested.

~patrick

[Matt_Huybrecht · Accepted solution]

Hi Patrick,

John is correct - the Shell needs to be added further down in the model tree and the plenum is in the wrong location. I've modified your model and re-attached it here to give you some additional guidance.

A couple additional points here:

1. When you create a Shell feature, by default the system tries to shell ALL the geometry that is present in the graphics window. This means that the flange geometry with the holes on the front, the mounting flange, the ribs, EVERYTHING is trying to be shelled, The system ends up appearing to "hang" as it tries to do all the computations to solve the geometry. You have to consider the order of how you create things. In your model I suppressed that front flange and holes to eliminate them trying to be shelled, and I created the Shell feature BEFORE the ribs and mounting flange.

2. I would strongly recommend removing the rounds as being part of the sketch for your Revolve and Blend features. This is causing the tangency to be incorrect at the intersection of the Revolve and Blend features, and is causing me to not be able to specify the correct round value at that transition. I've attached the first few features of this model without the rounds so you can see how much easier it is to add the rounds/edit their values after the fact. In an ideal world you want to keep the sketch as simple as possible and leverage the Round feature itself to create the round. Notice also that I held off on creating the flange until AFTER the Shell feature.

Regards,

Matt Huybrecht

[pb_max]

Hello Matt and John,

That helped.  However, TO ME, the problem I encountered remains a question.  There has to be a way to shell a solid portion of a model.  Otherwise the feature is useless on ANY complex model.  This model isn't even that complex!!!...do you see my point?  In the file I attached, SO WHAT if i shelled a different portion?...I should be able to shell the part that is built later as well.  This is a very real world scenario, as at my company (and everywhere, really), the first iteration is nowhere near what the final model is.  It is built upon, over and over again.  If I add some knob or fin or big scoop on design step 57, and need that thing to be shelled, I need to know that I can.  So - what is the recommendation in both my attachment and real world scenario?  Add the thing as a seperate body and shell it, then combine the bodies later?

Thanks,

~patrick

[pb_max]

FYI I was able to update the revolve and blends to be body 2, subtract 2 from 1 (keeping bodies), then shell 2, and finally merge them.  At least I know it is possible.

[Matt_Huybrecht]

Hi Patrick,

The short answer is that there IS a way to shell a solid portion of a model and omit other areas of the model that you don't want to shell. This is done in the Options tab:

Basically, you have to select a set of closed surfaces to omit from the Shell. There are multiple ways to select surfaces, whether selecting them individually, using Seed and Boundary, using Loop Surfaces, and so on. 

To use this portion of the Shell feature requires you understand a bit about surface selection so didn't want to overwhelm you with information.

It is far easier to choose a design intent that puts the order of operations in such a way that you don't have to worry about omitting parts of geometry to get a successful shell. You are also asking the system to do more computation to calculate the solution so I expect this would probably increase regeneration time, too.

This is Design Intent at its core along with deciding which references to select, which constraints to use, how to dimension something, etc. You can always insert features and reorder features. As you noticed you can also use Multibody to achieve the same result. This is a different design intent choice.

Regarding recommendations, it's hard to give you any because I don't know your products. There are some fundamental principles that you should try and adhere to, however, with regards to your modeling practices. For example:

1. There is an order of reference robustness when it comes to selecting references for the creation of new features: datum planes/datum entities are the most robust, followed by surfaces, then edges, and finally vertices. The more robust the reference the less likely you are to experience failures when modifying the model.
2. Try to save creation of rounds until near the end of the model. Otherwise you're more prone to selecting rounds as references, and since rounds come and go you're likely to get more failures when modifying the model. It's a similar situation for draft features.
3. Never leave weak dimensions in a sketch.

Regards,

Matt

[pb_max]

Really excelent information Matt, thanks!  

[Matt_Huybrecht]

You are VERY welcome. I know you're frustrated but keep at it. The more you use Creo the more you learn kind of the right and wrong for how to do things. You'll get a sense for how it works. It's a tool that can be used to model literally anything, but that's also what can make it difficult to grasp because there's a lot to learn. 

Since you're a LEARN subscriber, I suggest taking the class on Design Intent for Part mode. It's called, Creo: Part Design Intent and Reference Management.

Also, we do have a ton of free tutorials in Learning Connector for many different aspects of Creo. We have curated groupings of tutorials to create playlists. We're trying to update these playlists so that you create your own dataset on your own Creo so that you can always refer back to them. For example:

• Get Started with Creo Parametric Modeling - You end up creating a tea kettle model as you go through the different exercises.
• Learn More About Creo Parametric Modeling - You create the beginnings of a drone assembly.
• Get Started with Creo Parametric Assembly - You continue with the drone assembly and assemble the components together to create the assembly.

The models are simple but hopefully help give you some additional practice and help.

As your company upgrades to a newer version of Creo you might want to learn about all the new enhancements. You can use Learning Connector to watch videos of all those enhancements. These are created by the Creo Product Managers. I believe you are on 9 when I looked at your model. So when your company updates to, say, Creo 11, you might want to know all the new Assembly level enhancements in both Creo 10 and 11. You can find those here.

Hope this stuff helps!

Matt