Parametric Asssembly

[Anonymous]

I want to make a parametric assembly from a kind of tank we use a lot. It should be all seperate parts in an assembly. Number, angle, heigth and size of nozzles are variable. I have side and roof nozzles. Also Diameter and heigth of the tank is variable. Roof can be flat or an angled. What would be the best approach to make an assembly that i can reuse. Or maybe top down moddeling so all parts features become solids... (have no experience with that neither)?

[Mark.Lancaster]

@Anonymous 

My 2 cents..   I would go the iLogic or VBA route.   You could do an iAssembly if you don't know programming but going this way, the iAssembly may get to complex and a nightmare to manage.

[SharkDesign]

iLogic is definitely the best way if you are making loads of different ones, but will take a lot of time and knowledge to setup properly.

Otherwise, copy design if you have Vault is very useful.

[Frederick_Law]

Master sketch.

Setup all parameters that will change: Tank Height, Tank Diameter etc.

[Anonymous]

So, I undersand that a part is the best way to go, and not the assembly way. I preferred the assembly way, so I could have a partlist with the different flangesizes in it.. 😞

@Frederick_Law 

So sketch up all possible flanges/sizes too?

[johnsonshiue]

Hi! I agree with the experts. Without using iLogic, the best workflow would be skeletal modeling (multi-solid body or master sketch). With iLogic, you can choose between driving parameters from the top-level assembly or you can use iLogic rule to drive parameters within the master part).

Many thanks!

[SharkDesign]

Another option is linking all the parameters to an Excel sheet. Never had
good luck with this though and it usually breaks at some point.

[Frederick_Law]

I used Master Sketch in assembly since IV 5.3

Still using it in SW2019.

I don't like multi-body part.

Too many body counts 🤠

MS control most parts in assembly and location for all purchased, CC parts.

You can have MS control all manufacture parts and add flanges and pipe to the assembly.

Or use iPart and iAssembly with MS.

[andrewdroth]

Hi JD,

I've made a lot of tank models like that over the years and my preferred method is a multi-body master part.

Depending on how many nozzles there are I will set up a spreadsheet that mimics the nozzle schedule on the drawing and drive the elevation, orientation, and projection values from that.

I usually start with a multi-body sheet metal part to make the shell, roof, and floor courses/panels. After I'm finished doing a 'Make Component' to push the bodies to parts in the assembly I convert the nozzles and other non-sheet metal parts back to normal parts.

For laying out the nozzles I have a dedicated plan sketch for each one that dictates it's orientation. From that I develop an elevation sketch to establish elevation and projection of the nozzles. From those I can make cut profiles for the sheet metal cut command.

All of the driving parameters are named and keyed (And sometimes linked to a spreadsheet as mentioned). The names are usual like "N1_ANGLE", "N1_ELEV", "N1_PROJ".

Here's an example I created recently. I've attached the pack and go project as well. This one is a little different than yours, but the process is very similar.

I've been meaning to make a YouTube video describing the entire process, but it's going to end up being pretty involved and I've been putting it off. Maybe I should dust off those notes.
 

[andrewdroth]

@jdg072 

Below is an example of how robust the final model ends up being. 

As long as the nozzles end up cutting the same parts everything works out, if there's a revision that requires a nozzle to intersect with a different shell part you just modify the solid selection in the Cut feature.

[Anonymous]

Great work! That's kind of tank I was looking for. Many thanks for the project files.

[andrewdroth]

No problem, I'm glad to help. 

[Anonymous]

I do need to find some tutorials on that Master Part design concept though 🙂

And how do you handle if you need 2 or 3 similar tanks in 1 project file? rename all files?

[andrewdroth]

Depend on how similar they are. Usually we would finish one to the drawing state, then use Vault to copy the entire project to a new folder with a name modifier like "-02" or whatever the equipment number was. It seems to be the best way to reduce re-work.

[IgorMir]

I would suggest - looking  into iParts and iAssemblies as well.

Cheers,

Igor.

---

@Anonymous wrote:

I do need to find some tutorials on that Master Part design concept though 🙂

And how do you handle if you need 2 or 3 similar tanks in 1 project file? rename all files?

---

[lena.talkhina]

Hello @Anonymous  !

Great to see you here on Inventor Forum.

I see a lot of interesting answers here in the thread. Did you find a solution?
If yes, please click on the "Accept as Solution" button as then also other community users can easily find and benefit from the information.
If not please don't hesitate to give an update here in your topic so all members know what ́s the progression on your question is and what might be helpful to achieve what you ́re looking for. 🙂