Parametric liquid tank

[gvidal25G2F]

Hi,
I'm trying to perform a parametric tank with Inventor. The problema that i have is that i dont know how to make to insert the nozzles on the tank totally parametrically: I want to have the parameter to change the flange and the pipe, and I also want to be able to adapt this pipe and flange to the Surface of the tank, and if it would be posible make the hole between them. 

By now i have the main form of the tank parametric and i also have my flanges that includes the pipe, I've put there the parameter to change the DN of the flange and also there is the option, when i insert it from my Content Center, to define the diameter of the tank so the pipe on the flange adapt on it. The problema is that when i need to change the DN, on the assembly, by right button, change diameter, I lose the parameter of Tank diameter and I'am not able to change it without reincerting the flange again.

There are a better way to work on it or i should keep working on this way?

And how could i make to insert the hole on the tank automatically when I insert the flange?

Thanks

[johnsonshiue]

Hi! Many thanks for sharing the information! I don't think I fully understand your request. Do you mind sharing an example (image or files)?

Thanks again!

[Anonymous]

Hi, 

I want to make a hole on the tank automatically when I insert the flange on the assembly, and if i move the flange by moving or rotating make that the hole moves automatically. Then, I also want that the parameter of the tank diameter to be referenciated with the flage, that for the moment i insert manual on the flange when I insert it.

Thanks for your help!

[Anonymous]

Are you trying to make this model with iLogic or Forms?

Is the tank drawing used mainly for visual parts (commercial drawings) - here the holes in the tank may be left behind.

Or is the drawing be used to manufacture this tank in the shop detailed drawings?

[SBix26]

With some extensive programming, this could be accomplished.  However, there is a different way to do this that you might consider.

Master modeling creates the parts as separate solids within one master part file, and these solids are derived to separate individual part files which are then brought together in an assembly file.  The master file controls the geometry and location of each part.

Using this technique, you would have the tank and flange defined relative to each other in the master file, using parameters for tank diameter, flange diameter, flange thickness, mounting hole diameter and qty, flange location, etc.

Once this is done, a change to tank diameter is simply a matter of opening the master file, making that parameter change, then updating the assembly-- that quickly, all parts are updated along with the assembly.

It is certainly possible to automate this to some degree with iLogic or other programming, so that you could select a flange # from a list, and give its location on the tank, which would then create the new flange in the master model.

How variable are the tank configurations you're working with?  I could also imagine having several different master files created for different numbers of flanges, which could then act as templates for starting a new tank, with parameters used to control each flange's size, location, etc.

Hope this helps to imagine some different ways to tackle your problem.

---

Sam B
Inventor Pro 2019.3 | Windows 7 SP1
LinkedIn

[andrewdroth]

I agree with @SBix26, I'd go the master part route for this.

Years ago I made this part that roughly does what you are looking for. Although this was for creating FEA models of API tanks the idea is the same.

I created a nozzle table in an embedded excel sheet and linked the parameters to sketches in the part. The nozzle features are suppressed by default then an ilogic rule check if the nozzle has been renamed in the excel sheet and un-suppresses the features if it has. The only downside to this approach is you need to define the maximum number of nozzle you might encounter ahead of time.

But it would work just as well for a solid body master part.

[gvidal25G2F]

By now i don't use any programing form, I've just used iparts. This drawing is for manufacturing, but it can also be used for comercial things.

Thanks!

[gvidal25G2F]

Could be possible to do something like this but instead of using a part file, using an assembly file? 

I would like to be able to make the list of the flanges automatically by detecting it

[admaiora]

I don't know if this is the same case. But definitively you can manage some case parametrically a fluid with iLogic.

[andrewdroth]

@gvidal25G2F  Absolutely.

Once you set up your solid bodies in the master part, you use 'Make Components' to push each body to a derived part in an assembly. After that, you just use the master part to update the assembly.