vessel design - general design question

[Anonymous]

I went through number of posts related to vessel design and was not able to find anyone asking following:

When you have a vessel/tank with multiple nozzles as well as internal members - baffles  or partitions, how do you go about modeling this complicated item? Do you go with multi-body part or start as an assembly from the get-go ? I am assuming that if it is done as multi body part, once design is completed, it would be derived and made into assembly (still new in Inventor and not sure how deriving works) ?

I am working on creating template files for us where we have 20+ different sizes of the same product, so not sure where to start. Al i know that i need to set the foundation properly...

thanks

[JDMather]

If you use a master multi-body solids file - go to Manage>Make Components to push out the individual part files and the assembly file.

[jhackney1972]

This is a personal decision but I thing the best method is maybe a hybrid one.  Start out with a multi-body design and along the way you can created an assembly from it using the "Make Components" command (see attachment).  This routine will automatically handle the deriving process for you plus the assembly will be linked to the multi-body part drawing.  This means that you an edit the multi-body part drawing and the assembly will update.  You can suppress or break the link at any time.

Once you have an assembly you can add parts that you have modelled separately or even design new parts, that can be adaptive if you wish, within the assembly environment.  One thing you want to avoid is modeling "features" inside the assembly drawing unless you have a very special use for them.

One thing you will be doing is borrowing geometry from other components in the design.  For example, fitting a baffle to the ID of the tank.  This can be done in the multi-body part or creating the part within the assembly.  If you do it in the assembly, the feature and part will become "Adaptive".  You might want to brush up on this Inventor tool before it bites you.

At the end of design, make sure you lock down your assembly by suppressing or breaking the link to the multi-body part.  Suppressing is a two way street but breaking is final so be sure which one you use.

As a SolidWorks user forced to use Inventor, you will soon learn it is just as powerful and versatile.  Good Luck

[Anonymous]

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@jhackney1972 wrote:

.... using the "Make Components" command (see attachment).  This routine will automatically handle the deriving process for you plus the assembly will be linked to the multi-body part drawing.  This means that you an edit the multi-body part drawing and the assembly will update.  You can suppress or break the link at any time.  

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This is quite helpful. Thank you.

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@jhackney1972 wrote:

One thing you want to avoid is modeling "features" inside the assembly drawing unless you have a very special use for them. 

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Not sure i understand what you are saying here. Do you mean modeling based on the sketches saved in the assembly itself (not contained within a part)? Or something else...

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@jhackney1972 wrote:

One thing you will be doing is borrowing geometry from other components in the design.  For example, fitting a baffle to the ID of the tank.  This can be done in the multi-body part or creating the part within the assembly.  If you do it in the assembly, the feature and part will become "Adaptive".  You might want to brush up on this Inventor tool before it bites you.

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I intend to take care of these items through multi-body part. I am assuming that it will be easier to control it that way.... and that's how i would do it in SolidWorks as well

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@jhackney1972 wrote:

At the end of design, make sure you lock down your assembly by suppressing or breaking the link to the multi-body part.  Suppressing is a two way street but breaking is final so be sure which one you use.

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Need to brush up on this one too 🙂

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@jhackney1972 wrote:

As a SolidWorks user forced to use Inventor, you will soon learn it is just as powerful and versatile.  Good Luck 

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It is difficult to transition. After using inventor for a while now, i still do not understand why certain features were done in certain way. Really makes no sense. I am not doubting that inventor is not powerful software package (and rather cheap). From my own experience SolidWorks is way more intuitive and easier to get into. With Inventor you have to know how certain design is achieved by digging through tips and tricks, and workarounds... that is all. 

Thank you for your input.

[andrewdroth]

Multi-Body all the way.

I make plan sketches of all the nozzles, baffles, ect., then elevation sketches based on those. 

By changing a few key dimensions I can modify the position of most components, with very few issues. 

The only time you really run into a problem is if a cutout for a nozzle existing in the wrong body once you rotate it, but that's an easy fix.

Avoid adaptive parts like the plague.

Push the bodies to parts, pattern as often as you can using parameters linked from the master part.

Place downloaded\library parts as you normally would.

See Screencast. 

[Anonymous]

Andrew, thank you for your help.

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@andrewdroth wrote:

Multi-Body all the way.

I make plan sketches of all the nozzles, baffles, ect., then elevation sketches based on those. 

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 Can you explain this a bit more? Not sure if i understand it correctly.

I was leaning towards multi-body part. But i have an idea of doing all of my main skeleton (wall, nozzles.. ) as surfaces. This way it will be easier to manipulate nozzles and openings. Otherwise, it is a mess with all nozzle extrusions that would need to be cleaned up at the end..

[andrewdroth]

The ScreenCast below should illustrate the idea.

Essentially the plan sketch only controls the orientation on the nozzle. The elevation workplane/sketch defined with the orientation line from the plan contain all the information for creating the nozzle, and the cuts for the shell and to make the nozzle flush (if needed).

Sometimes I will create a block of a generic nozzle elevation, place it in the sketch, explode it, then constrain to origin and edit as needed. This can really speed up the modeling time if you have a lot of nozzles.

[Anonymous]

Thanks @andrewdroth for creating this screen cast. I was thinking about this in more/less same direction, but I was actually hoping that someone has a better idea on how to go about this. Have you thought about creating 3D sketch instead of your plan sketch? that could possibly be easier (more conveniently ??) controlled... Don't know. In any case, thank you for your help !!

I am going to try with surfaces to see how that one goes first.

Cheers