Trouble with parameters and rectilinear patterns

[IBNobody]

I am trying to recreate this object as a parameterized model, but I am having trouble with patterning. As you can see, it has vertical slots that vary in length based on the curvature of the outer circle.

I can create a rectilinear pattern of the 2-corner rectangle in the sketch, but when I go to extrude, I always have to select the faces to extrude. (This is how I got the original picture.) Thus, adding in parameters that change how many copies are made in the pattern operation breaks the extrude.

I can create a rectangular extrude cut from a rectangle with corners tangent to a sketch circle and do a rectilinear pattern on the extrude. While this works better with parameterization, the new cuts don't respect the tangent.

Is there a better way for me to go about this?

[jhackney1972]

Please attach your model so the forum users can take a look and troubleshoot your issue.  If you do not know how to attach your Fusion 360 follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save to your hard drive. Then use the Attachments section of a forum post to attach it.

[IBNobody]

Here you go.

[jhackney1972]

Try again, I do not see the attachment.  Check to see if you see it attached to the bottom of your message before sending.

[IBNobody]

See if that came through on the previous post.

[IBNobody]

Another thing I tried was to create rectangles running in the X axis, use the rect pattern, create more rectangles running in the Y axis, and combining the output. (Note that this is not the pattern I'm aiming for, but I was experimenting to see if I could figure it out.)

I found that changing the rect. pattern instance count broke the combine step (hence the extra uncombined bars on the left and right). This isn't going to get me where I wanted either.

Is what I'm trying to do breaking down because parameterized models don't play well with pattern placement?

[g-andresen · Accepted solution]

Hi,

Adjust option is your friend.

Screencast

günther

[g-andresen · Accepted solution]

Hi,

Another one

Screencast

günther

[IBNobody]

Ah, so the problem I was running into was caused by a few things that you solved @g-andresen .

1. I was extruding the rectangle upwards from an XY sketch rather than from a XZ or YZ sketch.
2. I was trying to extrude a rectangle using total distance. You instead showed me that I had to extrude twice, with each segment set to extrude-to-object.
3. I was using the extrude-join method rather than the extrude-new-body method, which combined the extrude with the outer ring; not what I wanted.

This solved my initial problem, but now I am left with a bunch of bodies.

I can select all the bodies (the ring and the newly formed slats) and combine them into one body, but every time I change the number of patterned objects to create, the combine feature breaks. Is there a way to select all bodies created by the pattern feature programmatically/parametrically?

[g-andresen · Accepted solution]

Hi,

I don't see an easier way than this.
But you can try to make the beams longer and connect the pattern outside the geometry with a connecting body so that they become one body.
Then cut off the protruding parts with the boundary surfaces of the central part and hide them in the browser or remove them with "Remove".
But I think the first way is easier.

günther

[IBNobody]

I suspected as much. I'll make it work with touching the combine command at the end after adjusting my parameters. Thanks!

[IBNobody]

Taking a similar route, I thought that if I reduced the size of the cylindrical lip and used it as a boundary for cuts, I could get my desired object without the pattern selection issue I stated previously. (One cut body vs multiple bodies.) I tried to pattern the extrude/cut so that I would only end up with one object. I set the extrude to the following, and the extrude looked correct.

But the pattern operation (with adjust) didn't keep the extrude direction the same. (It extruded to the right face, just not the face I wanted.)

Is there a quick fix to this, or is this a limitation with the adaptive-pattern/extrude-to-object feature?

[g-andresen · Accepted solution]

Hi,

In fact, it is also for me (at the moment) a behaviour that cannot be explained.
Maybe @jeff_strater can take a look at it?
In the screencasts I show processes for parametric arrangements of slots and square cutouts.
In the attached files you can also follow the process step by step.

günther

Slot parametric

Square cut out parametric

günther

[tanwinghoe1983 · Accepted solution]

This looks like a job for the web command. Each subsequent patterned web feature will respect the tangency.

Wing Hoe

Fusion 360 School

https://www.youtube.com/channel/UCU7QDqWAeIdCK5aNFXPgX2g