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?

[etfrench]

You can edit the name of any dimension.  Clicking on the star will add it to the Favorites section of the Parameters dialogue.

[RogerInHawaii]

I know that I can give a name to a User Parameter and that I can also change that name later.

But that's not what I'm asking about.

I have a sketch that I'm editing. I use the Dimension tool to add a dimension to some line or between two lines or points. This puts a dimension kind of "callout" right onto the sketch. Doing that does NOT automatically create a User Parameter for that dimension value. Is there some way that I can tell Fusion to use that value for a new User Parameter, and to ASSOCIATE that User Parameter's value with the Dimension (measurement) within the sketch?

Yeah, I could COPY the dimension value, pop up the Parameter dialog, and add a new, named User Parameter and give it that value. But that does not ASSOCIATE the User Parameter with the Dimension on the sketch.

You say that "You can edit the name of any dimension value". But that doesn't seem to be true. You can edit the names of USER PARAMETERS but not "Dimensions on a sketch". In fact, it appears that you cannot simply give a name to a Dimension on a sketch.

[mavigogun · Accepted solution]

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@RogerInHawaii wrote:

Doing that does NOT automatically create a User Parameter for that dimension value.

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Yes, it does- it just doesn't put it where you might intuit looking for it.   You can find the Parameter in the Sketch section.    Check it out:

 

[jeff_strater]

@RogerInHawaii, the answer to your question is no - you cannot create a User Parameter when creating a sketch dimension.  There is an item in our backlog to be able to name a sketch parameter on creation, but that will just be a shortcut to what @etfrench suggested.  I'm curious, though:  what do you see as the value from a User Parameter over a named Model Parameter?

[etfrench]

The key take away is sketch dimensions and other automatically created Model Parameters can be used exactly like a User Parameter.  Changing the name and adding it to the Favorites makes it even easier to use.

[mavigogun]

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@etfrench wrote:

The key take away is sketch dimensions and other automatically created Model Parameters can be used exactly like a User Parameter.  Changing the name and adding it to the Favorites makes it even easier to use.

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Exactly!   Knowing that every Dimension received a name (D1, D2, etc), it stood to reason those names could be replaced.    Apparently, a developer thought so too, made it so. 

[lichtzeichenanlage]

In addition to what @etfrench said:

• The key difference is, that user parameters are true global and model parameters are kind of focused on a component. If they're marked as favorite they are globally accessible but if you copy/past new a component than Fusion 360 will automatically rename all model parameters in the copy to e.g xxx_1 and keeping the favorite marker. This makes it easy to apply different values. 

[RogerInHawaii]

Thank you, one and all, for the informative replies.

I was unaware that/how dimensions become automatically named and placed into the Model Parameters list.

Whenever I would bring up the Parameters dialog the Model Parameters section is, by default, not expanded. It never occurred to me that some things might end up there automatically since I never saw anything in that list, precisely because the default for that section is to NOT be expanded. Once I DID click on it to expand it I indeed can now see that a while slew of parameters, each name starting with a 'D', resides there.

Still, it's definitely awkward, when I'll want to name a dimension that I've just added to a sketch, to have to ALSO open up that Parameters dialog, find the recently added one in the Model Parameters list (presumably the LAST one in the list), and change its name. It would be REALLY NICE if there were a way right when I'm adding the Dimension callout, maybe a pop-up field that shows the default (e.g. D99) and lets me change it as necessary. OR, perhaps allow me to right-click on the just (or any previously) added Dimension and show the Name and allow it to be edited.

ALSO, when I DO have the Parameters dialog up, it would be REALLY HELPFUL if clicking on any of the Model Parameters would result in the corresponding object (e.g. the Dimension callout from which it was created) were highlighted in the sketch. Right now I've got a whole bunch of those Model Parameters but have no way of relating them to the Dimension callouts that created them, so there's (now) no way for me to give them reasonable names.

[TrippyLighting]

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@RogerInHawaii wrote:

Still, it's definitely awkward, when I'll want to name a dimension that I've just added to a sketch, to have to ALSO open up that Parameters dialog, find the recently added one in the Model Parameters list (presumably the LAST one in the list), and change its name. It would be REALLY NICE if there were a way right when I'm adding the Dimension callout, maybe a pop-up field that shows the default (e.g. D99) and lets me change it as necessary. OR, perhaps allow me to right-click on the just (or any previously) added Dimension and show the Name and allow it to be edited.

ALSO, when I DO have the Parameters dialog up, it would be REALLY HELPFUL if clicking on any of the Model Parameters would result in the corresponding object (e.g. the Dimension callout from which it was created) were highlighted in the sketch. Right now I've got a whole bunch of those Model Parameters but have no way of relating them to the Dimension callouts that created them, so there's (now) no way for me to give them reasonable names.

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While this idea already exists in the Idea Station section of this forum, yours is so well explained in its functionality and UI that it would be great if you could add it as an Idea to the Idea Station. You'd have my immediate vote!

[RogerInHawaii]

Thank  you for the compliment. My career was as a software engineer specializing in UI development. 

[lichtzeichenanlage]

You can hover over a dimension and it shows the name. But this is not a nice way...

If it comes to names I have two entries in the idea station. 

• Pulate names
• Add name field to dialogs

[TimeFramed]

Here's the problem I'm having.  I want to base something on the distance between two points in two different sketches.  So I created a third sketch and drew a line between two points.  The dimension of that line is what I'm after using as a variable (referring to it elsewhere).  But that fusion-generated dimension is not under the model parameters for the component that the sketch is in.  Even if I add a (driven) dimension, that also is not present.  ??

[etfrench]

Set the dimension equal to a User Parameter.

Can you post your Fusion 360 file?  There may be a better way to accomplish what you're doing.

[TimeFramed]

I might be able to post an older save of the model.

The "better way" was to define the parameter value (height of a "peg"), and then use that to offset the sketch plane from the "base plane" of the peg.  Then that I could use that parameter later (for the mating peg).

During the initial design, I originally created the top plane for the peg a sketch as an offset plane of another surface (i.e., so the top of the peg was relative to that surface).  Doing so, however, meant that the only way I could "know" the peg height was to measure the distance between the planes (or two surfaces in those planes).  So that's what I tried to do; I created a "measuring" sketch that simply had a line perpendicular and between the two planes.  In doing so Fusion calculates and assigns the dimension, but that dimension is not in the parameters; no sketch section under that body.  I tried, then, adding a dimension to that line, which of course was a "driven" dimension, since it's predetermined, and fixed.  But even that manually-added driven dimension does not show up in the parameter list.

In the end, defining the peg height was really the correct way to approach it anyway; I just had to back up the timeline, and redefine that original plane offset to be offset from the peg's base plane, and use the peg-height variable as the offset... and then go repair the things that broke as a result of that change (e.g. redefining sketch planes and lost projections -- and redefining one of the planes moved the entire sketch; presumably due to the original plane's origins having being rotated relative to the model's origin, and not the other, ugh.).

It would have been more convenient if I could have captured that dimension, eliminating the repairs.  (though admittedly, having the peg height done right is better, and maybe I'll be better at thinking ahead more in the future. 🙂

[TimeFramed]

I don't have a saved version showing the problem; just the one before I ran into the issue and one after I did it the "right way".

But it's easy to reproduce. Attached is a file with 3 sketches. Sketch 3 contains a dimensioned ellipse, and a line coincident with the other two sketches' planes (length 7mm).  Fusion sets the dimension for that line, and I can add a driven dimension to it (which I did), but neither are available in the parameter browser.  I was wanting to find that driven dimension, give it name, and refer to it; either in another parameter, or directly in features (e.g. extrusion).

[davebYYPCU]

Every input you give a Fusion Model, will have it listed under the feature you add it to, 

You were looking for the distance between 2 planes, it's right where you put it.

Can be renamed, and assigned as required.....

Might help.... 

[TimeFramed]

Dang!

(and thanks!)

I guess I was just looking in the wrong place.

Now I really wish I had my actual model file to find it there.

I *thought* I had opened up everything in there looking for it *somewhere*, and didn't see it, Ugh.

[TimeFramed]

Not to beat a dead horse, but I tried something closer to the sequence of events in my actual model, and seem to have a driven dimension that does not appear in the parameters.

You can see the sequence of events in the timeline.

In the last sketch, I projected the center points of the other two sketches' circles (which fixes them), and then drew a line between them.

The length/distance is 34.134 (and the driven dimension only appears while editing the sketch).

There is a 19.134 which was the offset plane distance (from the top of the box).

I'm thinking the value 34.134 is not (directly) present in the parameters, because it's being derived from 15 + 19.134; i.e., distance-z (the height of the extruded box) + the AlongDistance (the plane offset of the plane of the top sketch). 

This was the scenario I ran into; I was after that 34.134 value (in this example) in a variable.  Now, if I had known where to look, and found the appropriate values going into the computed distance, I could have (renamed the contributing values, if desired and) made a User Parameter that combined those sub-values appropriately to get the distance measurement I was after.

Again, thanks for the help, and now I'm pretty sure I *did* look everywhere for that value. 🙂

[davebYYPCU]

Looked but not seen.  Its all here and all makes sense,  D3 + D6 = Driven dimension

Your offset plane comes off the top of the box.

So yes we are on the same page so far, what is it you want to do, Height = D3 + D6.  User parameter can be done, but will still give the driven dimension only.

Might help....