Solid Body Palooza!

[MRanda]

I have seen a post similar to this where the writer wished the ability to access the visibility of a solid body via iLogic. I am asking for the ability to suppress via the solid body. As things are now, if I want to suppress a solid body, I have to suppress every feature within the body separately! When doing this via iLogic, it creates a mess! Currently I may be forced to suppress dozens of features –and I I add new ones, I need to remember to add those to the code as well. 

The multi-solid body layout part workflow is easily the most powerful design paradigm in Inventor, but the ball was definitely dropped on this one. It was thrown out there and immediately orphaned. We should also have the ability to:

• Add iProperties to the solids that will transfer to the part. Color, Material, Cost, and all of the rest.

• Ability to organize solid bodies to groups –which become assembles when the “Make Component” command is evoked. Ability to suppress an entire group!
• A visual indicator of which solid body a feature belongs to would be nice as well. It’s hard to organize a feature tree, but any focus on that would be a help. We finally got folders in assemblies after years of requests, it’s about time to look into cleaning up a parts tree as well. For instance, I put ALL sketches before features (projected geometry is all sketch to sketch –far more stable). I would like to be able to group and hide them. There can be thirty or forty of them and the tree gets incredibly long!
• Attaching iLogic that would survive the “Make Components” process and become a rule on the other side would be killer as well.

I’m sure I’ll come up with more. Have a great day!

Mark Randa
Applied Design Intelligence

[VdVeek]

This question is asked here once in a while. I think it's not the right use of the multibody option when you want to have different materials for different solids. You create only different solids but it's still in the Part environment. When you place a Multibody part in an assembly what material do you want to see in the Bom? A part can only be shown as one item/component, handle it that way. 

If you want to have different materials for the different solids use the make Components, that's the way inventor designed it.

Rob.

[jtylerbc]

I agree with VdVeek as to the original intent of how multisolids were intended to be used.  However, there are some situations that could be handled more easily with the ability to assign materials to the individual solids.

For example, it is common at my company for us to download supplier models to use in our assemblies.  Sometimes these are assemblies in the real world, but don't really have any moving parts (think of something like a steel fitting with rubber O-ring seals).  For convenience, we will import these as a single part.  In the current system, we have to set the material for the combined part to the material that makes up the most of the part.  This causes the weight of many parts to be slightly exaggerated.

For the case where you are going to use Make Components to turn the multisolid into an assembly with parts, the resulting parts could inherit the solid's material, providing a central place to edit the materials.

I don't think the two concepts are mutually exclusive.  In fact, it seems somewhat odd to me that the entire point of Layout Parts and Multisolid Modeling is to have a central part file controlling an assembly, but that master part is not currently permitted to control the materials of the resulting parts.

[dan_szymanski]

Hello, thanks for the suggestion, however this Idea was previously logged here: http://forums.autodesk.com/t5/ideas/v2/ideapage/blog-id/v1232/article-id/5682  AND here:  http://forums.autodesk.com/t5/inventor-ideastation/solid-body-palooza/idi-p/3755426

As such I am setting this Idea to Duplicate.  Please be sure to visit the Master Idea and cast your kudo to it as to not split votes.  Thanks! -Dan

[timdown73]

I will be upgrading to 16 soon (we had a huge delay this year in update for tech reasons).  Have any of these multisolid improvments been implimented? 

[MRanda]

Hi Tim. I would likely hold off on updating to 16. I am finding it VERY slow compared to 14. Likely culprit is the multi-solid bodies in sheetmetal parts. I have an iLogic model that takes over two and a half hours to run that should take ten minutes or-so. The only differance between this and similar models is the use of multi-solid body sheet metal parts and the use of 2016. I skipped 2015 because of performance problem, and should have skipped 2016 as well. 

To answer your original question, no, nothing has been done.

Mark Randa

Applied Design Intelligence

[timdown73]

Thanks for the reply and update MRanda!

[rogmitch]

Hi Mark,

In the hope that IV 2016 had improved solid body suppression I was trawling the web and came across your post.  As you remark things are no better regarding suppression but at least patterning solid bodies is now much easier!

In trying to circumvent the problem, I first thought of suppressing individual features but as you mention this is a messy road.  The solution I devised after some trial and error  is to create a solid body part model (e.g. SB1.ipt), save it and then create a copy part with a modified name (SB_Final.ipt) .   In SB_Final.ipt delete out all the solid bodies that you need to be configurable.  Then derive in the same solid bodies from SB1.ipt and these bodies can now be accessed from the model tree in the ilogic browser and suppressed in the  usual fashion via 'Feature.IsActive'.

 Changes to the configurable part need to be made in SB1.ipt to prevent errors on suppression but I think this is a small price to pay for the overall ease and control you have over the solid body model.

You may already use this method but I thought it might be helpful to outline the method for anyone with the same problem.

Roger Mitchell

[MRanda]

Hi Roger,

Not sure that I fully understand your workflow, but any port in a storm if it is working. This idea was accepted long ago, yet there has been no action taken. I'm beginning to think the 'Idea Station' is like the office suggestion box that drops directly into the waste basket -- they hope you will just forget about those pesky ideas over time. At any rate, glad things are working for you!

Mark Randa

Applied Design Intelligence

[rogmitch]

Hi Mark,

I can only agree that it is a real shame that AD have not tackled the limitations of solid body modelling in the last few years.  From my perspective (using IV since v5) solid body modelling is by far the best approach for static models and yet I doubt it will ever gain the popularity it deserves until the clunky workflow is fixed.

With respect to my workflow,  just derive a solid body from one part  to another and then try and suppress the solid body in the receiving part. You will find it is possible.  Go figure!

Roger Mitchell

[DRoam]

For anyone interested, I've posted another Idea requesting some other improvements to multi-body parts. It's mostly targeted at iParts, but also addresses issues related to multi-body and derived parts, such as how work features and patterns survive the Derive process (spoiler: right now, they don't).

You can read the idea and give it a vote here: Improvements to iParts, Multi-body, and Derived Parts

[DRoam]

Regarding the "Add iProperties to the solids that will transfer to the part. Color, Material, Cost, and all of the rest."... please see the conversation that took place in the comments on @bverboort's related idea here: Multi-Body iProperty Support.

There was some very productive conversation about how that might be implemented as well as some other needed multibody/part configuration functionality.

[dan_szymanski]

Idea added to backlog for future consideration [433 & 434]. Thanks!

[Silvia.van.Emmerik]

Suppressing solid bodies in Inventor with ilogic is especially a great idea for FDU assets, see

https://forums.autodesk.com/t5/factory-design-utilities-ideas/speed-up-inventor-assets-by-suppressin...

[alain_miltenburg]

Agreed, there should be a simple iLogic function for that.
In the mean time you could use some basic .NET functionality for controlling Solid visibility in one line of code per Solid:

Option Explicit On
Option Strict On

Dim surfaceBodies = CType(ThisDoc.Document, PartDocument).ComponentDefinition.SurfaceBodies.Cast(Of SurfaceBody)

surfaceBodies.FirstOrDefault(Function(x) x.Name = "1stNameToFind").Visible = True
surfaceBodies.FirstOrDefault(Function(x) x.Name = "2ndNameToFind").Visible = True

 
This could even be made shorter when omitting the two Options and removing the CType(). But my finger refused to type that. 🤓