topic Sheet metal thickness parametric in Fusion Support Forum

Sheet metal thickness parametric

Anonymous — Wed, 30 Aug 2017 12:30:13 GMT

I seem to be unable to use a "user parameter" as the input for a sheet metal rule. Consecutively: I seem to be unable to use the thickness of a sheet metal rule I made as a parameter or dimension elsewhere.

This makes it very difficult to match sheet metal components with other types of components parametrically.

Am I missing something? Or can I go ahead and post a feature request?

Re: Sheet metal thickness parametric

kate.raskauskas — Wed, 30 Aug 2017 15:23:22 GMT

Hi @Anonymous,

I think the sheet metal rules can't be driven by parameters because sheet metal rules are global and parameters are locally defined. Would making a few sheet metal rules and picking the rule based on the current parameter work for you? For example, something like this that might help match more easily with parameters:

Re: Sheet metal thickness parametric

Anonymous — Fri, 01 Sep 2017 12:00:41 GMT

Hi Kate,

Thanks for the explanation! It is similar to my current workaround. I have marked 'sheet metal' parameters so I'm reminded to change the rule as well.

However, it kinda defeats the purpose having parameters. To me, the whole value of parameters is that I can change model geometry based on rules in one place. I don't want to have to go and change a bunch of sketches and rules too.

About the global / local conflict: I wouldn't know anything about that. Sheet metal rules are listed as "in this design"? I as the user am blissfully unaware of such distinctions, and can only comment on what I think would be useful / user friendly. Having parametric sheet metal thickness to me would be very useful.

Re: Sheet metal thickness parametric

JBerns — Sun, 10 Sep 2017 16:57:02 GMT

This would be especially useful when creating extrusion cuts.

Instead of a typing a value, it would be much easier if we could type "Thickness" for the extrusion distance and Fusion would cut the extrusion equal to the thickness of the sheet metal rule assigned to that body/component.

I see that in the Parameters dialog box, you can mark each sheet metal rule Thickness parameter as a Favorite, However, d0 or d5 are not useful names. You could rename these favorite parameters to associate them with the sheet metal rule. For example, the thickness for 'Steel (mm)' could be "SS_025mm" and 'Aluminum (mm)' could be "AL_0200mm".

Fortunately, we have auto-complete available to assist with the long names. The challenge though - if you change the rule assigned to the body/component, and it uses a different thickness, then you must edit all the extrusion cut features to use the new parameter. Had it just referenced the "Thickness" parameter from the rule, it would have been much easier to change the design.

Holes and cuts should be able to easily access the Thickness of the sheet metal rule assigned to the body/component which is being edited.

Regards,

Jerry

Re: Sheet metal thickness parametric

Anonymous — Mon, 15 Oct 2018 17:39:57 GMT

How to add those parameter ? And everytime for different sheet metal thickness we supposed to add new one?

Re: Sheet metal thickness parametric

Anonymous — Thu, 25 Oct 2018 02:02:01 GMT

Thanks Jerry,

Your words :

" I see that in the Parameters dialog box, you can mark each sheet metal rule Thickness parameter as a Favorite, However, d0 or d5 are not useful names. "

Your words gave me an idea to use the auto generated parameters in a reverse way,

I mean i can use the auto generated named parameters (we could rename it) to represent the sheet metal rule Thickness as a parameter. for me it is a good solution for now.

Regards,

Maher

Re: Sheet metal thickness parametric

brad.micallef — Sat, 01 Mar 2025 02:30:08 GMT

I have a multi drawing assembly, and am using a master project file for all of my global parameters and sheet metal rules. Each time I create a new component (in a separate drawing file to reference in the assembly), I perform an INSERT DERIVE to bring in all those global parameters and sheet metal rules.

In this way, the sheet metal rules can be shared across multiple drawings but still be managed in one location across the entire assembly.

Regarding how to reference the component's sheet metal thickness attribute, based on the rule assigned to the component, I did the following:

After creating my first flange, I created a sketch and then a DRIVEN DIMENSION that references the flange thickness.
This DRIVEN DIMENSION (d39 in my case) may now be refenenced locally by the component sketches and formulas.
If the sheet metal rule is changed in the master file, or the assigned sheet metal rule for the component is changed, the d39 valriable will update automatically.

[AUTODESK]

- Creating global parameters, sharing sheet metal rules, and referencing a components' assigned sheet metal rule attributes (thickness, k factor, bend radius) should be MUCH easier than all these work arounds, marking favorites, insert derives, etc.

Brad M.