Rectangular pattern won't create more than 10 holes on either axis

[andrew2085]

I'm using rectangular pattern to create a grid of holes. The preview shows the holes in the correct locations, but after hitting Ok to close the dialog, only a subset of the holes are created. No error is displayed. The problem pattern is the last one in the timeline.

[andrew2085]

If I change the grid from 14x14 to 15x15 it does create the 15th holes on the border of the part, so it seems like it's just not creating the holes on the 11th+ grid squares for some reason.

[andrew2085]

I found the issue. I originally had the parameters grid_x_cnt and grid_y_cnt set to 10. These drive the patterns. When I changed them to 14, the 11th+ grid squares were created as new bodies which is why the hole pattern didn't create holes in them. The 7th item in the timeline, the extrude joins all bodies into one body. For some reason this doesn't automatically get recomputed when changing the parameters or explicitly changing patterns in the timeline before the extrude. When I edited the extrude and hit Ok it recalculated and joined the new grid squares and the holes are now correct.

Is this the intended behavior? It seems like a bug. I tried "Compute All", but it didn't recompute that extrude until I did it manually.

[johnsonshiue]

Hi! This does look like a bug to me. However, the condition leading to the bug is quite unique. The Extrusion11 is the culprit. The extrusion has dual purposes. It not only lengthens the outer frame but also joins the individual square pieces. It looks like the list of bodies to be joined was not updated after the number of pattern instances has been changed.

In this case, the square pieces should have been one solid body instead of individual solid bodies. If the base board was created first, followed by the square piece pattern, this issue would not have occurred. This is a bug but I am not sure how we could fix it easily. Let me work with the project team to understand it better.

Many thanks!

[TheCADWhisperer]

@andrew2085 

I would say your third step in the Timeline is done incorrectly.

This creates a bunch of bodies while it appears to me that your true Design Intent is to have one body?

I would say your technique is not logical.

[TheCADWhisperer]

@andrew2085 

I didn't take the time to set up the Parameters - but something like the Attached which more closely follows real world logic (with "cheats" available to digital techniques) is how I would model the geometry.  I start out with a base of material - just like in the real world.

[andrew2085]

It might not be how you'd build something in the real world, but it should still work and does work except when the bug is uncovered. I'm not sure how Fusion is handling feature dependencies and updates that leads to this, but in my head it seems like it should be something like this. 

When a parameter is updated or a feature is modified:

1. Create an empty "modified features list"

2. If this is a feature modification add that feature to the modified features list and start at the next feature in the timeline. If this is a parameter update, start at the first item in the timeline.

3. Does this feature use the modified parameter or have references to a feature in the modified features list or perform some operation on a body created or modified by one of the features in the modified features list? If yes re-calculate the feature and add it to the modified features list.

4. Run step 2 for the next feature in the timeline until there are no features left.

With these rules step 3 would see that Extrude11 performed an operation on bodies created in the modified features list (joined bodies created by features in the modified features list, Extrude8, R-Pattern4, and Extrude10) and would recalculated it re-joining the new bodies created by R-Pattern4.

[TheCADWhisperer]

@andrew2085 

It occurred to me that only one sketch is needed and it can be significantly simplified

to just a single rectangle and a line and some point locations for the holes.  (See Attached.)