Can I give a name to a sketch dimension?

[RogerInHawaii]

I know that I can manually add User Parameters and give them names. It's an incredibly powerful feature that I use all the time, because changing any User Parameter causes all sketches and objects and components that are defined by those parameters automatically get updated appropriately.

But suppose that I have added a dimension on a sketch. Is there any way that I can then give that dimension a name, so that effectively it becomes a User Parameter? I know that I could just manually copy the value of that dimension and go to the User Parameters dialog and add it as a new named parameter, but that wouldn't actually ASSOCIATE that parameter name with the sketch measurement. If something changes on my sketch that causes that dimension to change the User Parameter that I created from it would NOT automatically get updated since it really has no association with the sketch diameter.

So, IS THERE A WAY to have a measured dimension on a sketch and THEN associated a User Parameter with that measurement?

[GRSnyder]

Driven dimensions are not referenceable. They don't have names and don't appear in the User Parameters list.

This is a longstanding point of friction for a lot of people. Unfortunately, adding this ability is harder than it looks. I can't speak for Autodesk, but judging from past history, this isn't something that's likely to be fixed anytime soon. 

[TimeFramed]

Unfortunately, I've run into this same problem again.  This time, however, this time, the computations are not so simple.  I'm sure I could figure it out (fusion did) based on the raw inputs... (adding the length of the two values indicated by the green arrows to the "gap" value) ... but I really need to just be able to reference that driven dimension.  Computing those two values to add (based on the circles' radii and the connector_width) is not trivial.

Unfortunately, fusion is not storing this driven dimension in a 'd' variable, but is (apparently) computing it "on the fly".

The only values in the parameters are the "raw", simple, values.  I should not have to then make a user parameter that computes that dimension... fusion already did... but I have no way to get at it.

I think that *any* driven dimension, that I specifically call-out in a sketch should be added into the parameters.  At least at that point, I can find it, rename it if desired (most likely), and then easily refer to it.

[lichtzeichenanlage]

The line below the marked one should have the same length as the marked one? Use the equal constrain for that. If you want that both lines are symmetrical to the center line use the symmetrical constrain and both lines do have the same length. 

[davebYYPCU]

Why is that dimension important?  There are many ways to skin a cat.

Where are you going with that?  

Is the fx 22.00 going to be deleted?

That line is / can be fully constrained without being dimensioned. (Unless you delete the fx 22 dimension)

The measure tool will save that measurement to the clipboard, for use elsewhere.

[davebYYPCU]

He has mirrored that line.  Question I have is what to do with the referenced dimension if it is a driving dimension.

[TimeFramed]

Because I wanted to reference the dimension of that line elsewhere, so that another feature would be based on that dimension.

[davebYYPCU]

I think you will find a few requests in the Idea Station for this functionality.

It’s certainly a topic discussed here before.

[ToddHarris7556]

In short:

Driven dimensions cannot be used in formulas. 

In more detail. 

As a side note, they're also not exposed via the Parameters dialog, although they do get assigned a dXX name internally. 

As @davebYYPCU points out, if all of the inputs are available as parameters, and the driven relationship is quite simple, it can be possible to 'reconstruct' the driven value in formulas. In VERY SIMPLE cases, this is true. Unfortunately, one of the most useful applications of driven dimensions is in simplifying formulas. 

This is not an 'everyday' pain point, but it's certainly an annoyance for those of us coming from Inventor who are used to using reference dimensions in that way.  

[GRSnyder]

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@ToddHarris7556 wrote: This is not an 'everyday' pain point, but it's certainly an annoyance for those of us coming from Inventor who are used to using reference dimensions in that way.  

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It's an everyday pain point, provided that "every day" means "at least weekly". 🙂 I find myself coming up against this again, and again, and again... The problem is that there's no viable workaround. The cases where you can easily compute the relevant value by hand aren't the cases where you really want to reference an existing dimension.

[denyerec]

It galls me that this was from well over a year ago and is still not implemented in any form. In Inventor one could just type: myParam=20mm into the dimension creation callout and boom, a parameter was created. Using Fusion is akin to pulling teeth, the UX for dimensioning is perverse.