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Changing the units of a user defined parameter does not work.

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Message 1 of 8
Julie_7
186 Views, 7 Replies

Changing the units of a user defined parameter does not work.

I was so excited to notice that in the parameters dialog that I can now click on the units for a parameter and change the value. I often forget to change the count of something to have "no units".

 

I just created a new design, opened parameters and added

- x_unit 50mm

- y_unit 50mm

- x_units 1

- y_units "no units" 1 which made me realize that I had forgotten to change the units to none for x_units.

- So I clicked on units for "x_units" and changed it to "no units" and it changed the expression to "(1 mm)/ mm" which seemed strange. I then changed the expression to 1.

- When I went to use the parameter in an expression for a length in a sketch it failed. (x_units * x_unit). By failed I mean the expression was red and I could not save the value.

 

While recreating the issue for this writeup, I found that I can only change the units in the parameter dialog before the parameter is used somewhere.

 

Regardless whether I leave the strange "(1 mm)/ mm" expression, or change it to be just one, the parameter is treated in the sketch as if it had units and the expression is invalid.

 

More information:

- If I then change from "no units" back to mm the expression stays unchanged as "(1 mm)/ mm" which is incorrect. However the value which had been "1" now changes to 10.00 which is even worse.

 

I am using Fusion 360 2.0.17954 x86_64

 

7 REPLIES 7
Message 2 of 8
jhackney1972
in reply to: Julie_7

When you change the units from mm to No Units, Fusion 360 can only do one thing to fix the units and that is add the / (divide) by 1mm.  If you remember from your basic algebra class, to remove units, you divide by 1 of the unit, in this case 1mm.  This is normal.  When you want to change it back to mm, then your change the units and "you" must remove the "/1mm" from the expression the expression value to 1mm. 

 

As far as changing units after a parameter has been used is not possible.  Fusion 360 must preserve its integrity of used units or your sketch would lose definition.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 3 of 8
Julie_7
in reply to: Julie_7

@jhackney1972 

I think you missed the critical part of my post. I should have made it more clear. Sorry.

 

   


@Julie_7 wrote:

Regardless whether I leave the strange "(1 mm)/ mm" expression, or change it to be just one, the parameter is treated in the sketch as if it had units and the expression is invalid.


What I was intending to identify as not working:

I thought that changing to no units just after creating the parameter was a time saver and better than deleting the parameter and starting over. However, after changing it to no units, when I later try to use the parameter in an expression that fails because F360 does not treat it as a unit-less number.

 

In addition, although you are correct that to remove units dividing by 1 mm is correct as an expression, there is no reason not to then cancel the units and show the result as just "1" in the expression. That might also be part of the fix for the above bug.

 

Message 4 of 8
TheCADWhisperer
in reply to: Julie_7


@Julie_7 wrote:

That might also be part of the fix for the above bug.


Can you Attach a file here that illustrates this "bug"?

Message 5 of 8
jhackney1972
in reply to: Julie_7

I can see your issue now.  In the video I replicate it when I change an inch user parameter to No Units and then try and use it in a Circular Pattern.  Until this is looked at and fixed, I offer a workaround in the video.

 

@Phil.E , I wanted to call your attention to this please.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 6 of 8
Phil.E
in reply to: jhackney1972

Thanks. This is known and some solutions are being discussed. (FUS-138728)





Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.


Message 7 of 8
Julie_7
in reply to: jhackney1972

John:

I woke up this morning thinking about your comment about changing units.

"As far as changing units after a parameter has been used is not possible. Fusion 360 must preserve its integrity of used units or your sketch would lose definition"

1. If units is changed to "no units" when the expression is not compound, there is no benefit to keeping the units in the expression (1mm/mm). Just change the expression to "1". This is obviously what I want.
2. Even after a parameter is used, changing the units should be allowed within the same class (length, angle, etc.) as this does not change the stored value which is always in cm and therefore none of the model calculations are affected. If the expression for the parameter is just a literal value when the units is changed then just converting the literal to the new units and putting that in the expression is likely what the user wants and should not cause any problems. (For example, if I have a parameter with units as mm and expression as 1000, then changing units to meters can just change the expression to 1.)

A related though about units...

For any design the default units must be specified. However, when there is a need to enter a value in different units, it would be nice to have the option to display units as entered, or as noted in the parameter list.

While writing the above paragraph, I did some experimenting and realized that how it works now, and what I am used to, is not what I would consider logical.
Example:
I draw a rectangle on a sketch and enter 10 for the height and 3" for the width.
I open the parameters and go to that sketch and find that both height and width have units set to mm (the design default) and the value of width is 3".
I would find it logical that implicit parameters would get created with units set to the default if units are not specified, but with units set to the specified type if that is specified in the field during the sketch.
In addition, if I go to the trouble to specify non-default units for some dimension then I might expect that that is important information and the units should be shown on the sketch for that dimension.

Of course, this might just be the ramblings of a computer programmer who is not an expert in CAD. 🙂
Message 8 of 8
Phil.E
in reply to: jhackney1972

Thanks again for reporting this.

 

The major release that came out yesterday has this fix. Please give it a try and let us know if all the cases are solved now! (build 2.0.18719)

 





Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.


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