Adaptivity

[AnthonyHarris90842]

I use an assembly file and then I add multi body parts to it and then model new solids in these multibody parts.

I use adaptivity a lot as I use the various multibody parts as references for ther parts.

My problem is that Inventor keeps loosing reference geometry even when I do absolutely nothing to the referenced part.

See attached pic.

Also I can be working on this assembly and all is good, then I close inventor and reopen the assembly file and I find that the geometry that I just redefined is lost again.

I am using Inventor 2021 and this version is the worst its ever been.
I am at my wits end and just about to cancel my subscription with Autodesk.
The Adaptive feature really needs loads of work as its never been great since the start and seems to be getting worse.
How can we get Autodesk to look at this problem?

[johnsonshiue]

Hi! Without seeing the actual Inventor files, I can only speculate. I suspect that you projected hole edges from a frame member. Then the frame member spec was changed and the source hole geometry was gone. Is that true? Please share an example that exhibits the behavior from scratch.

Many thanks!

[gcoombridge]

@AnthonyHarris90842 I've never had much luck with cross-part associations. In my experience they limit flexibility and slow performance. At worst they significantly degrade stability. Top-down modelling just seems to be unreliable in Inventor (and most other CAD platforms) 

The only time I consider it is when adding bolt holes to frame generator members. Even then, I project a part sketch curve instead of a model edge. 

I prefer to derive important sketches and work-features between related files or from a base Skeleton sketch.. This method is rock solid.

Sorry, probably not helpful but that's my 2c anyway.. 

[SharkDesign]

Adaptive parts are a fantasy. They are the perfect solution but frequently break. The general advice is to not use them at all if you want stability. 

[AnthonyHarris90842]

Hi Guys
The file set is massive as it is a full machine that I am doing.
What I am trying to find out is that are other people also having this problem.
As I said I have had in in many other assemblies too.

Gcoombridge as you say you have not had much luck with top down modeling.
I have used one multibody part to do a machine before which is more reliable but the file and feature tree becomes way to large so I then tried using more than 1 multibody part eg. one for the frame and one for rollers and then another one for other parts.
Also I noticed that if I project a work plane or axis from another part as reference geometry then that geometry is locked and does not update when I change the part where the work plane or axis resides.
I will do a smaller assembly so that I can post it on here.
I must say I enjoy the top down modeling and when it works its great and size wize its very reliable and also help a lot when I do the general assembly as I dont need to constrain everything and can just ground and root most parts unless they moving.

[SharkDesign]

I design machinery and wouldn't dream of trying to do it all in one part.

If you need to reference other things you are much better off referencing parameters. 

If you want to reference parameters across parts you can use ilogic to push all common parameters down from teh master assembly, this is the way I do it if everything is referenced. 

[AnthonyHarris90842]

Hi Jameswillo
Can you give me your method in steps or point me in the right direction to use Ilogic like maybe a tutorial
I have never used it before.
Thank you so much

[SharkDesign]

For instance, if I'm doing a conveyor I might run everything off the belt width. 

So in the top level assembly I'll have a parameter called 'belt_width'.

Every part inside that assembly is then driven by that width.

So a shaft would have the same parameter 'belt_width' and the length of the shaft would say something like d22 = belth_width + 80.

conveyor bed might be belt_width + 100.

Do the same with conveyor length, maybe you call it Con_Length. 

Once your assembly is all modelled you can control it from the TLAssembly. 

Change the width and length paramters and then run the code to push the parameters down. 

You can find an example of this code here from curtis:

Sending Parameters to Parts with ilogic - Autodesk Community - Inventor

You should just be able to create a new rule in the ilogic panel and copy and paste the code. When you run that code it will push the parameters from the top assembly to every part under it. (I haven't tried this particular code though so I'm sorry if that doesn't work.)

[AnthonyHarris90842]

Jameswillo

Yes I use parameters like that and then link to the part that has the controlling dimensions.
Also I must add this is not always possible depending on the design.
Sometimes I have to reference actual geometry and this is where Inventor falls short.

I wish that Autodesk works on only Adaptivity and if they only got this one feature right for the whole year we would all be very happy.

[robbeRtek]

Hi,

I've had the same problems,...

The solution is to not project things from a 3d solid. the red icon in an unstable reference, because when the complex model rebuild, some edges/solids disappear in that process and come back but with another id I guess.

you need green references.

When you need to project geometry use always work features or sketch lines to project.

And in the version 2021 : the ilogic copy don't work good with complex reference model assembly’s.

There are reference problems.

The solution is to create a new folder for each copy and  to copy directly to that folder.

Every copy in the same folder doesn’t work.

Robbe

[cadman777]

Yeah, and then maybe I can convert Inventor into a structural platform.

But first I'd have to be willing to sign-on to subscription slavery...

Dreams and more dreams!

[cadman777]

I've done conveyors and conveyor systems before and used a top-level sketch-part instead of a t/l assembly.

If the conveyor system is large, then I use 2 layers of t/l sketch-parts.

The top-most sketch-part has construction planes/axes/points and sketches for locating positions, critical widths and lengths, and it contains all critical parameters. That sketch-part is derived into all the down-line sketch-parts. So, the next layers of sketch-parts are for each assembly. For example: In a 3 conveyor system, there's 3 additional sketch-parts. That way the top-most sketch part is not HUGE.

I found that if I go any deeper than 2 levels of sketch-parts, Inventor bogs down to a crawl when getting into the finer details of the assembly and parts. I try to keep all the sketch-parts as simple as possible, and make all parameters as common sense named as possible. Plus, I try to reuse as much data as possible, and dare not use ANY surface geometry in those sketch-parts!

Also, the bad system overhead comes with the sheetmetal guards and fasteners, but that's another topic.

[AnthonyHarris90842]

Hi Cadman777
I found that when I use construction planes / user defined planes and axis these generate locked geometry instantly and dont update when positions change.
So far it looks like there is no solid elegant solution and that everyone has some work around method.
How can we get Autodesk to pay attention to this problem as it is a problem we all facing and costs us so much lost time when the parts lose reference.

I am pulling my hair out

[SharkDesign]

I think Autodesk are not doing anything because most users just know that using a lot of adaptivity is just bad practise. If you mate things properly, you don't need adaptivity because you'll know when the mate breaks that something doesn't line up. 

If you think about how many lines a single projection can be and then your assembly is full of projected adaptive geometry. Everytime you change anything it has to go through every adaptive sketch to see if anything has changed and then update it and then that could change another adaptive sketch to update, your computer would be so slow. 

[johnsonshiue]

Hi Anthony,

Adaptive is a powerful workflow. It works when things are properly adapted. However, when you establish an adaptive relationship, you want to make sure you clearly understand their constraint relationship (driver and follower). And, how the constraint will alter the geometry in what way.

In some cases, you may want to ground the adaptive part so that the sketch or the feature can adapt more easily. Another common issue users encounter in Adaptive is the cyclic relationship. Essentially, you have PartA drives PartB and PartB drives PartC, which also drives PartA. This kind of relationship can lead to confusing behaviors or endless update.

Please feel free to share an example that exhibits the painpoint. For the most cases, there should be a better way to do it.

Many thanks!

[cadman777]

@AnthonyHarris90842 

Please allow me to clarify.

But first let me say this:

I NEVER use Adaptivity b/c it is GUARANTEED to BREAK.

And it breaks mostly at the end of a project when I can't afford the time loss!

No more cussing and throwing things around, HAHA.

The work-flow I described NEVER uses Adaptivity.

Instead, it's using Derived sketch-parts.

IOW, I open a new part and derive the t/l part into it and use only the sketches and work features from the 'parent' part that are needed in the 'child' part. I ONLY go 2 LEVELS DEEP this way, so as not to kill performance.

I've done some pretty large assemblies that way (in Inventor 2010!), and never had any problems.

There's a lot of up-front work doing the Deriving, but 'that's life'.

If the design must change late in the project, I just change either the top-most sketch or the next one down that controls the relevant assembly or part. Then a Global Update fixes the whole assembly, including ALL dependent parts.

I NEVER, EVER use Adaptivity b/c it SUCKS!

It's a JOKE.

It's an ABORTION.

It should not exist in the software (like so many other half-baked functions).

Hope that clarifies.

Now, to answer: 'Does Autodesk care'?
Absolutely NOT.

All they give a s**t about is their g.d. revenues.

End of story.

"The love of money is a root of all kinds of evil."

[robbeRtek]

Here is another way to-do 🙂
With feature ‘make part’, every reference/work feature/parameter ect force down to each part.
And build the components with this references, and not with project geometry.
The components are all placed on the origin from the main assembly.
Robbe

[torbjorn_heglum1]

I stay away from adaptivity when it comes to design of structure. I recommend master models as described here: https://forums.autodesk.com/t5/inventor-forum/master-modeling-tips-amp-tricks/m-p/8795856

and have a quite simple, stable and robust way to do my designs top down.

Still I use adaptivity for routing in the assembly, ie tubes and cables. But according to strict rules -  only creating adaptive work features. In this case the adaptivity is carried over from the assembly to the part by constraints, so it can be traced and changed whenever needed. When the routing is completed, I turn off the adaptivity and suppress the constraints to reduce rebuild times and file dirtying to a minimum.

Torbjørn

[Anonymous]

I have used SolidWorks for years but an open position at a competitor requires knowledge of AutoDesk Inventor.  I did use Inventor for a 6 month stretch some years ago and was eternally frustrated with adaptivity.  Things that were easy to accomplish in SolidWorks, such as stable multiple step automated machine cycling, even if I replaced parts and actuators, absolutely didn’t work in Inventor without time consuming rework.

I came here to see how things progressed.  I think I’ll pass on the opportunity.

[AnthonyHarris90842]

I really don't know why Autodesk cant get adaptivity right.
We all have been asking for a fix for years and some users will tell you not to use it at all in Inventor