Referenced geometry not working

[g3sjbhb]

Hello,

I am new to Fusion and following the official self-paced tutorials. 

I have read the docs and tried other online sources but I am stuck with what is shown in this official video: https://help.autodesk.com/view/fusion360/ENU/courses/AP-INTRO-SKETCH-BASICS-CONSTRAINTS at 5:20.

The idea is simple, I am trying to reference a fillet using the dimension tool.

I know that the same result could be achieved using the equal constraint, but for the sake of sanity and understanding I want to know what I am doing wrong.

The steps I am undertaking, while in the Sketch workspace:

• create a rectangle 
• apply a fillet to a corner (A)
• apply a fillet to another corner (B)
• delete the auto generated dimension of B
• select the dimension tool
• select B 
• enter the prompt
• click on the dimension of A (Rx)

Expected behaviour:

• The value of A should become a "dx" that should be referenced from the B fillet dimension

Current behaviour:

• The fillet dimension of A is not being referenced

System:

• MacOS 12.4

I have attached a screen recording of this simple workflow. Would greatly appreciate any insight.

Thanks

[wersy]

That's what I've noticed lately as well.

[g-andresen]

Hi,

1. I tested it several times under W 10 and could not reproduce the behavior.
2. if it does not work under MAC after reboot, I would consult the Service Utilities.

günther

[TrippyLighting]

I cannot reproduce the issue on Windows 11. I might try later on my MacBook 

[g3sjbhb]

I have found the issue and I don't believe this is an intended behaviour of the software. Please confirm.

My Design History was switched off. When I switched it back on the references started working as expected. 

Another weird side effect of the History being switched off is that the custom parameters feature also disappear.

Please see screenshots attached.

  

[wersy]

Same problem with Windows 11

[TrippyLighting · Accepted solution]

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@g3sjbhb wrote:

I have found the issue and I don't believe this is an intended behaviour of the software. Please confirm.

My Design History was switched off.

---

That indeed IS the intended behavior when the timeline is disabled. This is Fusion 360's non-parametric direct modeling mode, so refencing the parameter of other dimensions is not possible.

[g-andresen]

Hi,

1. The behavior is to be expected because there is no parametry when history is disabled.

2. However, when history is enabled, assigning parameters during creation works for straight lines, but not for fillets and chamfers.
These require a subsequent transfer of parameters.

günther

[g3sjbhb]

Thanks @TrippyLighting for confirming. However, for my benefit, can you please elaborate on the relationship between the Design History and the parametric mode.
It is far from obvious why switching one on/off would impact the other as they both handle very different aspects of the software. I should be able to reference dimensions without having a backup of this action.
Thanks

[TrippyLighting]

Design history and parametrics are one and the same in Fusion 360 and most other mainstream parametric CAD software. The one exception I am aware of is SpaceClaim as that is a parametric direct modeler.

If you start developing a model in parametric mode an turn off the timeline, sketches loose their relationships to the geometry they helped creating. I would also believe that all connections between dimensions in features and sketches that are referencing parameters are cut and the UI fields are populated with the values rather than the referenced parameters. 

You can use direct modeling techniques in a parametric model by creating a base feature and then start creating geometry. That is an advanced topic I would not worry about at the moment.

[g3sjbhb]

Thanks for the detailed answer, much appreciated. 🙏

[TrippyLighting]

You are free to mark any of the answers as the solution 😉