Math Error popping up in Conditional Feature Suppression - Inventor 2024.3.5

[nathan_wostrel]

I will preface this with: I am running Inventor 2024, Build: 343, Release 2024.3.5  This issue is not due to the model, the error can be replicated by making any feature and giving it these parameters and conditional feature suppression. I do not want to upload this file, it has external references and is very complex.

I am running into an error with formulas in the conditional feature suppression system.  Here are the general parameters.

This error shows up in several instances, but I will just go over one of them. For this feature, I need the suppression to occur if SheaveInnerDiam <= HubDiam + HubReinThickness * 2.

As you can see above,

SheaveInnerDiam = 1.336 in

HubDiam = 2.5 in

HubReinThickness = -.582 in

If we do the math,

-.582 * 2 = -1.164

2.5 - 1.164 = 1.336

Therefore, the formula is equal to SheaveInnerDiam and the feature should suppress. However, it does not. I can only attribute this to an internal rounding error since everything is stored internally in Inventor in metric units. This formula works if the requirement is >=. I also tried "round(( HubDiam + HubReinThickness * 2 ul ) * 1000 ul / 1 in) * 0.001 in" and this works on features that need >= but not <=.

I am very confused by this error and would love some help.

Thank you,

@nathan_wostrel Your post title was modified to add the product name and version and to increase findability - CGBenner

[johnsonshiue]

Hi Nathan,

The behavior does not sound right to me. Either a parameter is also driven by another expression in the Parameters dialog. Or there is an iLogic rule override the behavior. Please share the ipt file here or send it to me directly at johnson.shiue@autodesk.com. I would like to understand it better.

Many thanks!

[nathan_wostrel]

I made a model with nothing but the example error. I knew this was able to be done as I had tried this already. It is not i-Logic or other driven dimensions, as there are none here. It is completely independent of the fact the original file has external references. There is a problem with how Inventor resolves numbers, at least in 2024.3.5.

Update: Found one of the computers in the office has 2024.3 and the behavior exists there as well.

Thank you,

Nathan Wostrel

[andrewiv]

I can confirm that I also see this issue.  It only seems to happen when using an unit other than cm.  Here is a very simple example where the properties of Extrusion 2 are set to suppress if Test1 is less than or equal to Test2.

If I use cm in my parameters the feature is suppressed.

But if I use inches then the feature is not suppressed even though the values are the same.

It has something to do with the units conversion and if there is a formula in the parameter because if I just type in the same value then it works.