Configurations & Emboss feature

[AlessandroZap]

Hi everyone,

Emboss feature seems to reach a limit with configuration feature.

In my design, I have a curved component with variable width depending on configuration.
The component has a an "EMBOSS" operation to emboss a sketch with rectangular pattern (slots) on his curved surface.
In the sketch, the pattern command has a parametric function that defines the number of the slots depending of the component width.

Now, when I switch from a configuration to another, it seems that the emboss command can't manage to select all the slots profiles created in the sketch. The results is that some slots are not embossed (but they are correctly calculated by the sketch). 

It should be nice if the Emboss feature had a "select all profiles" option in the sketch reference.

Any suggestion to solve this?

[TrippyLighting]

The "golden rule" for pattens is to keep them out of sketches. If you can share the design we can provide more targeted advice.

[AlessandroZap]

@TrippyLighting ,

Thanks for your reply. I usually keep patterns out of sketches, but how do you manage to pattern a a feature on a curved surface without emboss command?

I can't share the entire design, because it is property of the company where I work. I'll make a new one just with component needed. (I already attached a video to show what I mean)

[AlessandroZap]

@TrippyLighting ,

Here is an example design with the same features.

Thank you

[TrippyLighting · Accepted solution]

For whatever reason Fusion 360 takes an eternity to download the configured design, so I am sharing a video that explains the process.

1. I extended the sketch for the flange with a 1mm tangential line. 
2. Then I edited the flange feature and add that little line to the selection. That straight line will be used as the stationary feature in the next process. 
3. I use the Unfold feature in the sheet metal workspace to unfold the body into a flat piece.
4. I create a sketch and center the slot.
5. I use a cut-extrude to create a single slot in the center.
6. I create a (timeline) feature pattern with the appropriate settings.
7. I use the re-fold feature to re-fold the flat piece into the bent sheet metal geometry.
8. I trim off the little straight piece and use the remove feature to remove the unneeded sheet metal body.

[kgrunawalt · Accepted solution]

Yes this is a current limitation the emboss command,  not configurations specifically. There is a similar limitation to other commands that we are aware of that are especially noticeable in configurations.

The limitation is that the emboss feature only uses profiles that are explicitly selected which you have done. It does not accept the pattern as a selection defining the profiles where the pattern count can change and the emboss adjusts.

This limits what you can do with a pattern output parametrically. There are commands that are smarter about things like patterns. The fillet feature can track another feature like a pattern and fillet its output edges, adjusting as the pattern count adjusts.

But the emboss command doesn't yet do this. I tried selecting the profiles when the larger size was active but these profile selections are lost when the smaller size is computed. Strickly speaking, this is an emboss problem but it is especially noticeable in configurations.

The current workaround is to define an emboss feature per configured size and configure suppression of the feature so it the emboss for the size is only unsuppressed when the corresponding row is active. This is not ideal but it will work for now. I'll give it a try with your design and upload it.

[g-andresen · Accepted solution]

Hi,

try this

günther

[kgrunawalt]

I've uploaded the workaround. I had to

1. Modify the pattern count expression to be the largest size instead of using conditional (17)
2. Make sure existing emboss still just selects the smaller number of profiles from row 1
3. Suppress existing emboss in row 2
4. Create a new emboss for row 2, selecting all the profiles
5. Suppress new emboss in row 1

[davebYYPCU]

For as long as I have been here, downstream features can’t see the increased count items.

Works ok, when reducing the count.

The limitation is that the emboss downstream feature/s only uses profiles that are explicitly selected which you have done. It does not accept the pattern as a selection defining the profiles where the pattern count can change and the emboss adjusts.

Hardly an Emboss problem.

[kgrunawalt]

"hardly an emboss problem". That is why I said "There is a similar limitation to other commands"

[davebYYPCU]

Sure, saw that,

and this Strickly speaking, this is an emboss problem

it’s being addressed?

[AlessandroZap]

Thanks everyone for the contributions.
I understand that we are dealing with a little limit of the emboss command: sketch inputs have to be selected manually, but we can use one of the workarounds proposed.

@g-andresen I missed the final step: what did you put as input in the "rectangular pattern" feature?

[g-andresen]

Hi,

---

@AlessandroZap wrote:

@g-andresen I missed the final step: what did you put as input in the "rectangular pattern" feature?

---

This:

günther

[AlessandroZap]

Just to report another issue on this kind of workflow:

I adopted the solution proposed by @g-andresen because it was the faster and most effective.

In my design, I added another emboss feature after the pattern feature and an error occurred.
I understood that when you cut a part of a body that contains features pattern, something is miscalculated and you obtain a result like in the picture below.

Or worse in this case:

[TrippyLighting]

Did you try the workflow I suggested in my reply (message 14) ?

Did you run into issues with it?

[g-andresen]

Hi,

The behavior only occurs in context of the Deboss tool.
However, you can create the cut out without errors using the Extrusion tool.

@jeff_strater  Can you check that?

günther

[TrippyLighting]

@g-andresen for bugs, please tag @Phil.E 

[AlessandroZap]

The example I attached was a simplified version of my design.
In real life, I can't use the unfold command because my final component will be a double flanged and curved sheet metal body.


Actually, I'm working with a solid body for the curved version of my component (F360 doesn't allow flanges for curved sheet metal) and with a sheet metal body for the flatten version.

My design issues was related to the curved version.

That's why I couldn't use your solution, but that's my fault: I attached a non-full-representative example of my design. 

[TrippyLighting]

If you design this properly as a solid model, meaning with all the proper radii and all cut edges perpendicular to the main sheet metal surfaces and appropriate relieve cuts, you can convert the solid model to a sheet metal body, then unfold, apply the cut/pattern and then re-fold.

One area to be mindful of is to make sure you have a sheet metal rule in place for the specific thickness and materiel.

When converting a solid body into a sheet metal body, Fusion 360 picks the next viable option. Having the right sheet metal rule in place, reduces headaches.

Unfortunately, I don't have time at the moment to demonstrate this. 

Edit: Forget all that. Not that it is wrong, but it won't work with your model as you cannot design that with the current sheet metal tools in Fusion 360.

However, you can still apply a sheet metal workflow.

[AlessandroZap]

Yes, I know you can convert a solid body in a sheet metal body. The problem start when you have a "folded curve" like this:

In this case you cannot unfold the body. In real life, I use to cut multiple "teeth" in the curved flange in order to calender the sheet.

 

To make a curved unfoldable sheet metal body like this, I should use a kind of lofted flange with brake form, but that's not my purpose. I need a foldable sheetmetal body just to send STEP and DXF to my supplier.  Then I use Solid body for graphic purpose.

In other cases, when I don't need to unfold my component, I use the convert to sheet metal starting from surfaces. That's very useful sometimes.

Anyway, thanks for your time

EDIT: I just saw your edit 😄