Help with parametric pattern & combine

[keithd]

Within a component I'm patterning a body into, say, 10 instances. But the 10 is really parametric, i.e., the number of instances is computed from other parameters. This seems to work fine.

The problem is that for a further operation(s) on the resulting patterned bodies, I need to treat all of them as one entity. The convenient way to do this is to "Combine" all the bodies into a single body for the downstream operation.

But I can't find any way to make the selection of the patterned bodies parametric. For example, if I pattern the initial body and it turns out to create 10 bodies, I then go in and select bodies 1 through 10 manually, and execute the "Combine" operation. The problem, is that if I later change a dimension that creates a different number of bodies, only the 10 of the original selection get Combined as that is what the Combine operation in the timeline says to do.

What I need is some way to select all the bodies in the Bodies folder, no matter how many bodies are in it. Or some other way to make the "Combine" operation parametric.

Does anyone know of any way to do this?

Note, I know I don't really need to "Combine" all the bodies into one. But the problem remains if I want to treat all the patterned bodies, regardless of how many are created, as a single entity in a future operation, such as slicing them off at an angle with a construction plane. In the particular example I'm working on, I'm modeling a corrugated sheet metal wall. The most convenient and intuitively correct thing to do is combine the patterned bodies (which are repeated instances of one corrugation) into a single body that represents a full panel or a wall, the dimensions of which are parameters.

Thanks,

--

Keith

[g-andresen]

Hi,

1. show the process in a screencast.
2. Share the file and name the bodies, components and sketches involved.

günther

[jeff_strater]

there is no way to do that today.  Features which consume bodies do not have a way to specify "all bodies", or "all bodies produced by this pattern/mirror".

[keithd]

Thanks Jeff.

Seems like a needed feature. Hard to imagine it is not an often-needed capability. And it seems like a good goal to make all designs fully parametrizable. As is, the only workaround I see is to pattern far more bodies than would ever possibly be needed and then use a parameter-driven extrusion to cut off the unwanted bodies.

In thinking about it, the best solution I see is for the pattern tool to have an option to join the created bodies into one body. Clearly this is possible within the guts of Fusion, as Combine does exactly this. But putting that option in the pattern tool would be perfect because pattern knows what bodies it created.

It would be great if this could make it to a requested-feature list somewhere. Seems to me like it would be easy to add.

Thanks again.

--

Keith

[g-andresen]

Hi,

Why don't you show your design and say which body /feature it is about.
It would be possible to connect the 1st instance (feature) to a base body via the joint option and not create it as a new body.

günther

[keithd]

Because Fusion no longer gives me an icon for launching Screencast. When I launch it directly from the app icon in Finder the app will not let me sign in. It complains that I have no Internet connection, which obviously isn't true because I'm signed into Fusion 360 and I'm signed into this Forum to post this reply and I've been watching Fusion 360 videos on the Internet for the past two days trying to find a way to do what I'm trying to do.

But I'm not sure a Screencast would be that enlightening anyhow. What I'm doing is dirt simple.

I'm trying to create a wall of corrugated sheet metal. The corrugation pattern is simple (four faces in the core) and there is not a lot of wall, so I want to model it rather than messing with textures, which are always inferior except where performance is a problem.

To do this, I...

1) Created and activated a sheetmetal component.

2) Created a sketch of the core of the corrugation pattern.

3) Created a sheetmetal flange from the sketch and extruded it up to the height of the wall.

4) Used the Rectangular Pattern tool to repeat this core body across the length of the wall, and beyond.

5) Used the Combine tool to join all the bodies into a single body.

6) Split this body at the sloped roof line using an Offset Plane .

7) Split this body to match the length of the wall using another Offset Plane.

😎 Used Remove to eliminate the two bodies I Split off in steps 6 and 7.

So I end up with a corrugated sheet metal wall as a single body within a single sheetmetal component.

The problem I'm having is that the Rectangular Pattern tool is parametrizable, but Combine is not. So I cannot arbitrarily lengthen the wall, even though it is a parameter.

Perhaps there are better ways to create such a wall. But if they are not fully parametrizable then they don't fix my problem.

I didn't understand your suggestion "It would be possible to connect the 1st instance (feature) to a base body via the joint option and not create it as a new body."  But when I tried to think of other ways involving components and joints I didn't come up with anything that was either simple or parametrizable. The way I did it also isn't parametrizable, but it is at least straightforward and simple.

--

Keith

[g-andresen]

Hi,

I perceive that there is no accompanying information on the subject besides verbal information.

But technical communication requires more than words.

günther

[keithd]

"But technical communication requires more than words."

What? I was an engineer for 45 years. I know for fact certain that technical communication does NOT always require more than words. What it does always require, however, is someone that wants to listen. In this case, what I wrote is plenty for someone to tell me either that Fusion has no solution or to suggest an alternative construction that is a solution.

In any event, I would be happy to provide a screencast if Autodesk would fix its Screencast app so that I could.

--

Keith

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[g-andresen]

Hi,

---

@keithd wrote:

.. technical communication does NOT always require more than words. 

---

If that were the case, one might ask, why are drawings and various visualizations created?

günther

[TrippyLighting]

The only way around the semi-parametric nature of the patter  tool is to find a way to pattern features rather than geometry.

What we really need is a way to automatically combine the patterned instances with themselves, or with existing, selectable geometry.

However, because the pattern tool also can pattern components an option to auto rigid-joint the patterned instances to the 1st instance or a selectable other component would also be very helpful. In combination, those additions to the existing tool set are a bigger project and it might take a  while before we see that in the product.

[keithd]

Because there are complex issues that benefit from drawings or visualizations.

But the issue I've raised is simple. Drawings or visualizations are not need. They would only waste my time in creating them or yours in analyzing them.

The issue is that the operation of Pattern plus Combine on bodies is not parametrizable because Combine cannot be told parametrically what bodies to join. What additional information would a drawing provide?

What I'm trying to achieve is simple. I'm trying to model the corrugated metal skin of a metal building. Unless you're from another planet and have never seen a metal building, no drawing is necessary to visualize it.

If Fusion has the ability to model the skin of a metal building in a parametrizable way, I would appreciate your advice on how to do it, if you know. I posted here because I thought someone else might have run into this problem and found a solution. I failed to find one. Fusion has many ways of accomplishing things and I do not profess to know them all.

In any case, I have no interest in continuing a debate on the topic of the appropriate use of words, drawings, or visualization in technical communications. At least not on this Forum in this thread.

--

Keith

[TrippyLighting]

See if the attached model is going to help.

It uses a number of user parameters.

That is what I mean with utilizing a feature pattern as a workaround.

The resulting part is a sheet metal part that can be unfolded and re-folded.

[keithd]

>"The only way around the semi-parametric nature of the patter  tool is to find a way to pattern features rather than geometry."

Okay, well, I'm not sure I fully understand the nuances of "features" vs faces, etc., so I'm not exactly sure how to go about this. I'll try to do some more reading up on "features."

>"What we really need is a way to automatically combine the patterned instances with themselves, or with existing, selectable geometry."

Right. I suggested the Pattern tool simply have an option to combine the bodies it makes. Of course that would only work for bodies, but at least it would work for that case, which seems like the most important case where you would need to join the results of the pattern.

>"However, because the pattern tool also can pattern components an option to auto rigid-joint the patterned instances to the 1st instance or a selectable other component would also be very helpful. In combination, those additions to the existing tool set are a bigger project and it might take a  while before we see that in the product."

Yes, I can see how auto-joint would be a good option for components, and I can also see how it would be a big project. But the partial solution of just allowing Pattern to join bodies should be easy. Conceptually, all you have to do is have Pattern call Combine passing it the bodies it should join. Seems very simple to me, at least. And I think useful even if the auto-joint option were not yet available for components.

Thanks,

--

Keith

[keithd]

Thanks for the effort putting this example together.

But when I change the num+features parameter the Convert to Sheet Metal step fails due to a Missing base face. I don't understand exactly why it fails, but it does.

But even if there is a way around this, it seems like an extraordinarily complicated method because you have to model every aspect of the sheet metal in the sketch.

What I did was super easy. I just drew a simple contour line in the sketch and let the Flange tool do all the work of thickening, bending, and positioning according to its rules. Then I just Patterned that slice of sheet metal and Combined the slices into one big sheet.

Just on principle, it seems like sheet metal tools should be used to model sheet metal.

Any idea why your approach fails at the Convert to Sheet Metal step? Is there a way around it or will this, too, preclude parametrization?

Thanks,

--

Keith

[TrippyLighting]

---

@keithd wrote:

Thanks for the effort putting this example together.

But when I change the num+features parameter the Convert to Sheet Metal step fails due to a Missing base face. I don't understand exactly why it fails, but it does.

...

Any idea why your approach fails at the Convert to Sheet Metal step? Is there a way around it or will this, too, preclude parametrization?

---

I have no idea why it fails, but I deleted and re-applied the convert to sheet metal feature and now it seems to work.

---

@keithd wrote:

But even if there is a way around this, it seems like an extraordinarily complicated method because you have to model every aspect of the sheet metal in the sketch.

---

Oh, I completely agree. It is quite a laborious hack, but unfortunately this is the only workaround I have available. This method/workflow also does not always work, because there are situation where something cannot be just created as a feature that combines with a base shape ("join" is the default option in the extrude dialogue).

[manu.weyers]

Pattern copies do NOT join automatically, why? (i don't want to manually combine, because the number of copies is parametrized !)

[laughingcreek]

this pattern limitation is fairly easy to over come by patterning a feature that is set to join.  see attached.

[manu.weyers]

excellent! but a checkbox on the pattern properties would be wonderfull.
Thanks

[dhr_jakob]

wow, very nice solution thanks a lot!