parametrically defined workplanes in assemblies don't get updated!

[Anonymous]

So As the title says, I'm trying to define a fully parametric model where some working planes are defined as an offset to a plane from another part in the assembly using some parameters. but when I change the parameter the plane does not get updated. see the attachment for instance.

[johnsonshiue]

Hi! I guess you did not click Update button (lightning bolt button at the top) after you change the parameter value. If you want to update the model after you change a parameter value, make sure you check the box "Immediate Update" in the Parameters dialog.

Many thanks!

[Anonymous]

I did all of what you just said. please see the screencast.

[Anonymous]

I think I have figured the bug out. I think it is a bug because it doesn't seem logical. basically when you define a plane using offset from a feature (e.g. plane) of another part in the same assembly using a local parameter, the plane just gets the current value and ignores the later updates of that local parameter. but there is also a global parameter defined with the name flush<number> which updates the offset if changed. I don't know why Autodesk has done this. but it seems rather a bug than an intentional feature!!! 

[t_stramr]

Hi. Could you ZIP your dataset (parts and assemblies) and attach to your next post?

I can validate your findings and start appropriate process to fix this issue if necessary.

Thanks,

Robert

[Anonymous]

Due to the confidentiality of the project I'm not allowed to share files here, but I have tried to replicate the issue in the zip file attached to the main post. I have figured the issue out and I have also a work around. but it could be good idea if Autodesk Inventor team fix this supposed bug for the next versions.

[johnsonshiue]

Hi! I think I know where the problem is after watching the video you recorded. The issue here is that you are changing two user parameters, which do not drive anything. Did hese two parameters use to drive the workplanes? If yes, the relationship no longer exist after you make the workplanes adaptive. Adaptive workplanes are driven by the parameters associated with the assembly constraints in the assembly. If the adaptive workplanes are also driven by the user parameters within the part, there will be two drivers trying to influence the same object, leading to collision. Does it make sense?

Many thanks!

[Anonymous]

Johnson,

using different CAD software (including mechanical Desktop 🙂 ) this seems like a rather weird approach if not a bug. if I wanted to have a parameter in the assembly, well, I would make it in the assumably. I want to make a working plane inside a specific part using features in sibling parts, and Inventor just takes the current values of the parameters I give to it, and makes new assembly parameters and ignores further changes in those local parameters!!! I would strongly recommend the Inventor team to change this. I can't think of any practical situation where the current behaviour would be of any benefit. 

[johnsonshiue]

Hi! The behavior you are seeing is actually how adaptive works. I assume you created the workplane in PartA by dragging from a face in PartB, right? The issue here is that PartA and PartB are two separate documents. PartA isn't aware of the existence of PartB and vice versa. To accommodate the need to drive the workplane in PartA from PartB, Inventor uses "adaptive" technology, which stores the adaptive relationship at the assembly level and manages it as such.

The CAD systems which can establish inter-component relationship easily are usually having all components within one document. As a result, everything is in one context and everything is stored in one file. For CAD systems having individual component files, inter-component relationship will have to be managed separately, which could be unintuitive at times.

Many thanks!