Infer constraints turned off, yet constraints are still being inferred.

[kristin.jakuszanek]

Hey all!

I am having issues with how inventor automatically infers constraints. I have the setting for this turned off yet constraints still are being inferred all the time, whether I am in an IPT file, or IDW. 

Is there a known issues with this feature still functioning, even though the setting is turned off? Or are there forced inferences that cannot be turned off?

Also, I had read somewhere before that coincident constraints on edges don't show in the 'show all constraints', as to reduce screen clutter, but sometimes these coincident constraints that don't show are what's causing me issues. Is there a way to actually have inventor show all the constraints, regardless of how much clutter it will cause?Line automatically inferred constraint to objectInfer setting is turned OFFWhat shows with show all constraintThis is what I also want to see during show all constraints

[kristin.jakuszanek]

Johnson, 

I think I have it all figured out. I must ask though, what is the point of unchecking the infer button and it greying out the inferences? To me, when I was unchecking the infer box, I assumed all the greyed out options wouldn't apply, but they do. Now that I have unchecked all the options, they don't infer. Is the infer constraints check box just a way to lock in what constraints are being inferred so it can't accidentally be changed? Also, I looked, and as Igor had stated the coincident end constraints show as yellow dots, not as the constraint icons. 

I would love to be able to see the icons when doing a show all constraint, but the software is clearly just not set up to show all in the way I want. 

Regards, 

Kristin 

[Curtis_Waguespack]

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@kristin.jakuszanek wrote:

Johnson, 

... what is the point of unchecking the infer button and it greying out the inferences? To me, when I was unchecking the infer box, I assumed all the greyed out options wouldn't apply, but they do.

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HI @johnsonshiue 

I would like to understand this as well. As I mentioned previously in this thread, I don't ever pay attention to these settings... but I thought I understood them... however the point about removing the check from the Infer Constraints checkbox and it still inferring constraints if the individual constraints are still selected confuses me as well.

I know these settings have gone through a few changes in the somewhat recent past, but can you confirm that this is working as expected? If so can you see where new (and apparently existing ) users are not going to be able to get results with these controls as currently implemented?

Can we also agree that the help files are deficient in explaining how to get these controls to work for the expected results? 

Thanks, 
Curtis

[kristin.jakuszanek]

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Can we also agree that the help files are deficient in explaining how to get these controls to work for the expected results? 

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I would just like to agree with Curtis on this. I almost always try to google for an explanation or look in the forums for answers before looking at the information files Autodesk provides on their help topics. 

[johnsonshiue]

Hi Guys,

The behaviors have not been changed for a few years, if I recalled correctly. I need to follow with the project team and see if we have more clear definition.

Many thanks!

[kristin.jakuszanek]

Hi Johnson, 

Have you been provided any more clarification into how these settings are supposed to function/why they function the way they do, from your projects team?

Regards, 

Kristin 

[johnsonshiue]

Hi Kristin,

I need to double-check with the project team. They will get back to you. Before any further clarification, I believe my prior explanation still holds true.

Many thanks!

[shaoni]

Hi Kristin,

Thanks for reporting these issues!

Issue 1, you still can get constraints to be created by checking off "Infer Constraint". This is not expected. I made a video in latest Inventor 2020, I cannot reproduce your problems. 

• With both "Infer Constraints" and "Persist Constraints" checked on, you can get your sketch geometries constrained during drawing geometry, either with connected geometry, or with the one you scratch your cursor on. 
• With "Infer Constraints" checked off, you cannot get constraints being created during drawing geometry, except Coincident Constraints on connected points, and the constraints created by specific commands, such like Offset and Pattern features. I saw Curtis mentioned this type in previous reply. 
• With "Infer Constraints" checked on, and "Persist Constraints" checked off, you can infer constraints with geometry connected or your cursor scratched on, but these constraints will not be created, except Coincident constraints. This is the same result by pressing "Ctrl", when both option checked on. 

so, if you can still reproduce this issue, could you make a video and also provide us your Inventor version?  

Issue 2, you want to show all coincident constraints on connected points. The reason to hide them is to reduce the clutter on screen. We want to use the yellow square dots to ease your snapping on end points, also to show curves/lines are connected. However, we saw the issue if you have more than two lines connected, the dots cannot show enough information about numbers, until you hover on it. But not sure how often you need hover on the dots to check numbers. could you please post an idea about this request? or voted an existing one. The one below is similar.

https://forums.autodesk.com/t5/inventor-ideas/highlight-sketch-line-ends-with-more-than-two-coincide...

Thanks

Nina

[kristin.jakuszanek]

Hi Shaoni, 

I made a video, but I can't get my previous inferences of horizontal and vertical to happen. I think my issue had to do with the persist constraint button still on. It seems I can get it to create coincident constraints from points to lines, which I didn't think should automatically infer, but if all coincident constraints infer regardless this is probably correct. I did have issues with the constraints still inferring horizontal and vertical constraints, as shown in earlier photos on this thread, but that may be a separate issues in the IDWs specifically, and I will pay closer attention to this.  

If I can get the behavior I was experiencing before to recreate itself, I will document it and get back to this thread. 

I am currently running build: 330, release: 2019.4- date: Mon 04/01/2019
When I originally posted in this thread I was running an earlier build of 2019, so that may also have had something to do with the issues I was seeing when I first posted. 

Regards, 

[shaoni]

Hi Kristin, 

The video is nice!

Yes, coincident constraints to connect end points are still inferred, even when you checked off "Infer Constraints". Also you figured out the only way to not infer coincident constraints is to check this type off when "Infer Constraint" is on. To make it so easier to infer coincident constraints, (or mentioned it as "make it so hard to not infer coincident constraints"), the reason is to reduce un-closed loops, and assume in most cases connected end points are required. 

So this constraint behaviors differently with others. Please let me know if you have different opinions, and appreciated for any great ideas to improve! 

Thanks

Nina

[Z-K-O]

This is inexcusably infuriating program behavior. I am at work right now and about ready to scream because I can't get my splines to stop snapping their control points together, no matter how many "solutions" I try, making them entirely useless.

I have some strong words for whoever had that horrendous idea, but I'd rather this post doesn't get deleted.

[johnsonshiue]

Hi! Please calm down. I know you are passionate and Inventor's particular behavior offends you greatly. I am sorry. However, as a tool, Inventor isn't worth your negative emotion.

I am not 100% sure your issue is identical to the original one. Please share the example here or start a new thread.

Many thanks!

[Z-K-O]

Alright. Well the issue arises when I create control point splines in a sketch, say, roughly parallel, 8 inches long, and an inch apart for the sake of example. Then click and drag a control point from one spline anywhere at all close to a control point of another, or the endpoint of a line or curve. At this point, the program infers a coincident constraint between the control point being dragged and the other point. This results in the inability to hand-place control points anywhere near each other to get the desired curve (without resorting to dimensions, which take an unworkably long time to use as a workaround). The behavior is true regardless of what sketch or constraint settings I disable, or any modifier key presses.

What can I do?

[johnsonshiue]

Hi! This is an interesting find! It looks like a bug to me. For some reason, the Infer Constraint -> Coincident does not work on spline control points. It does work on other sketch points, but not spline control points.

I will need to work with the project team to understand it better.

Many thanks for reporting!

[Z-K-O]

Sure. Looking forward to the fix, thanks.