Use Driven Dimension as a Parameter?

[Anonymous]

Hello all,

I am wondering if there is some way to do this, to use a driven dimension as a parameter. As it is, driven dimensions do not appear in the parameters menu.

if you hover over a driven dimension, it gives you the dimension number (i.e. d22, d46, etc) but you can't use it in the parameters menu.

Here is what I am trying to do:

We make custom cases/shipping crates. I want to put in the L, W, H of a part, say 3 x 4 x 5, define thickness packing material, define part spacing, and use the resultant size to make the case.

Usually, I'd just say (in the parameters menu)something like the folowing:

CaseW = (PartL+(Packing*2)) to define the case width if there is only one part.

But in most of our cases there are several parts (most the same size, and some very different). So the math looks more like:

((Part1L+Part2L+Part3L)+((NumOfParts-1)*Spacing)+(Packing*2)) for individual parts

(((PartL*PartQty)+((NumofParts-1)*SpacingBetween)+(Packing*2)) for patterned parts

which is driving me crazy.

What I did was this: I made a sketch with L+W, using rectangular pattern. Then, I used a rectangle around and defined the rectangle as always being 2" larger than the pattern (I will attach a simple representation of what I am talking about). This way I can change the pattern quantity and the parts sizing and it should be able to quickly define the length and width of the case.

BUT - when trying to use the driven dimensions (like to define (CaseW=d22) when d22 is a driven dimension), the parameter window simply won't accept it.

I think I understand why this is - because if I were to try and change this driven dimenison in the parameter window, I wouldn't (and shouldn't) be able to. But that also means I can't use it - ever? That seems a little strange.

In the attached file, try to use d22 and d23 (the driven dimensions) to create a parameter - you'll find you can't. it gives an error - "Invalid string" - as if d22 and d23 aren't defined.

Does anyone have any ideas? Or do I keep using my (long) equations to define my cases?

Thanks!

[DavidChemist]

Any news on this? I want to model pair of timing belt pulleys and see what kind of sizes i can run at what separations with a belt of constant length.

[chrisplyler]

No news that I've heard.

Do you want your timing belt model to be driven on: defined belt length, defined pulley sizes / ratio, driven center distance?

Or on: defined belt length, defined center distance, defined ratio, and driven pulley sizes?

[etfrench]

There are many online timing belt calculators which will give  you that information.  I use a program called Gearotic.

p.s.  You can set another dimension to a driven dimension.  It won't update when the driven dimension changes, but it does allow you to copy the set dimension to the clipboard.

[TheCADWhisperer]

@DavidChemist 

You could do this 10+ years ago (reference driven dimension as parameter) in Autodesk Inventor Professional.

You could do this 10+ years ago (real time constant length belt - change center-to-center distance and/or pully diameter) in Autodesk Inventor Professional > Belt Generator Design Accelerator.

Can you imagine Apple releasing a phone as "next generation" an iPhone that couldn't do what their product did 10 years ago.

Can you image Tesla releasing a car as "next generation" an automobile that couldn't do what their product did 10 years ago?

[DavidChemist]

I was able to solve my issue with a belt length formula and some time in excel. I still eagerly await this feature being implemented someday for future needs however

[WeatherHill]

Maybe not very helpful or insightful, but you (developers) might want to talk to the Inventor team. Using driven dimensions with other parameters has been a standard in Inventor for many years.

I do see the complications that's already been underlined here and I am aware that Fusion 360 is not just a light-version of Inventor, but surely it must be possible to port the code over to Fusion 360, without having to reinvent the wheel, so to speak.

As I've said, the ability has been there for Inventor users for many years (I am a daily user of Inventor) and the usage of driven dimensions is invaluable in some situations.

So I hope this will be available to Fusion 360 users in the near future aswell.

Kind regards

Anders W.

[frankstardelux]

Hi Jeff,

I can completely see your point of view and I take my hat off to the Inventor solver. There's some unsung hero's out there because it deals with all the stuff that I throw at it and more.

But here's the thing, following on from what TheCADWhisperer wrote, it's all about the timeline of things. Autodesk is pushing Fusion360 pretty hard from a marketing perspective yet it's lacking functionality that existing products have had for many years. I guess what I'm trying to say is, if it's not ready for release yet, then Fusion 360 should be labelled as a "beta" - use it for what it is but it's not finished yet. So you can see why people are getting frustrated when they hear all this marketing jazz and then can't actually follow basic workflows.

[Anonymous]

To use what would be a Driven dimension as parameter reference. I would do the calculation myself using superfluous sketch geometry as a parameter, then use that to reference another parameter.. It seems illogical since the dimension exists already and is normally just a straight distance between 2 X,Y/Z coordinates.
The worst of it is; is that you can't reference a line length between 2 projected points in a sketch. even if you draw it yourself, it's immediately constrained so no chance of adding a dimension as a parameter (e.g Entering longitudinalAngleOfDangle=THIS would be nice)
Or change the annoying popup to have the option of "Make parameter" since it knows the points for reference already.
Basically if you need to parametrise any pre-existing geometry; your longitudinalAngleOfDangle will be lacking! As shown in the attachment.. 1 single sketch plane using Intersected references. 3D sketch results in the same problem.
So if anyone knows of a parametrised way to get the length for something like a rectangular pattern using that hypotenuse as the Extent then speak up!
Pattern along Path will snap its handles to points, BUT never updates if dimensions change, so what's it actually referencing?!

[yebyps]

Obviously one needs to reference driven dimensions. It's such a basic thing. I've seen references on this going back to 2018 with the team saying they realise it's really important and they are going to solve it asap. But still nothing.  I'm stuck on my present design (folding, leaning things with cords) without it. 

[Careless_]

yeah still not understanding why this hasn't been implemented.

the only thing that comes to mind is that it would break previous designs that didn't assign a "dXXXX" variable name to the driven dimension.

it really should have done this from the start, and just make it non-writable. at least that way other parts of the design can use the same value as a pre-calculated dimension that you can't declare yourself.

[BaischBCWHRU]

To add to this thread...

I'm trying to space Xcircles of diminishing dimension in Ycircle where the Xcircles are tangent to the same outer Zcircle. Their centers DO NOT share a common circle, their edge does. I want to reference the Driven Dimension which is the angle they each create. This thread says I can't. I had a glimmer of hope when I created a "phantom" component. I drew a circle with a bunch of lines where the angle between the lines "referenced" the drive angles from the original sketch. BUT! Fusion simply pastes the value, not as a Fx: 

Is this potential work around more possible to code/program than giving us what we really want? 

[TheCADWhisperer]

@BaischBCWHRU 

It probably would have been better to start a new thread and Attach your *.f3d file (done as best you can to illustrate the Design Intent).

[etfrench]

Like this:

[frankstardelux]

By the way guys, I'm loving this Fusion 360 advert. A cut down version of it keeps coming on every now and again, and I just couldn't help but leave a sarcastic comment.

https://m.youtube.com/watch?v=dLIkW9gR4VU

[frankstardelux]

@BaischBCWHRU, I'm trying to understand, are you suggesting a workaround that Autodesk could more easily program in that would fix our inability to use Driven Dimensions in general, or in the specific case of circles within circles?

[jeff_strater]

to all subscribers of this thread:  The Jan 18 Fusion update (v2.0.12157) now supports using driven dimensions within an equation, as long as the reference is in the same sketch as the driven dimension.

[Careless_]

"as long as the reference is in the same sketch as the driven dimension."

So if I want to use a driven dimension to create an extrusion, that's not even possible?

come on, @jeff_strater... this thread has been bleeding out for 6 years. why the poorly fitting bandaid?

[mark_honeth]

...and if you have the driven dimension referenced elsewhere, e.g. in another user parameter in the favorites list, it can't solve. So frustrating...

[Johan_kaare]

@jeff_strater  "as long as the reference is in the same sketch" - Why? Wouldn't it be just, like, immensely much more practical if it was possible to refer dimentions in other sketches? Dimention variables are allready unique throughout the Design right? 

[jeff_strater]

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@Johan_kaare wrote:

@jeff_strater  "as long as the reference is in the same sketch" - Why? Wouldn't it be just, like, immensely much more practical if it was possible to refer dimentions in other sketches? Dimention variables are allready unique throughout the Design right? 

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Of course it would.  But, it is also immensely harder to implement.  Today, the sketch solver itself can handle these references within the same sketch all by itself.  Once you expand the scope to include references to other sketches or features, then you have to re-design the way that parameters are computed, in that some parameters can not compute their value until the feature that creates the geometry that drives that driven dimension is computed.  So, for us, we had a choice:  Release this partial solution now, or hold off, for potentially a very long time before getting any kind of ability to refer to driven dimensions in equations.  I hope that someday we will be able to implement the more general solution, but I think there is enough value in the "confined to a single sketch" solution that it was worth releasing.  Do you disagree?