Hole Tool is a little cumbersome and creating a pattern with holes is buggy.

[TrippyLighting]

1. Once youve slected the hole dimaeter handel you cannot go back and change the references, b=ut have to leave the tool to get back to edit those
2. When you o get back one of the references is wrong.
3. Finally when creating a hole pattern, even thoug the original hole goes through both components and despite th fact that both holes are slected the pattern is generated only in one of the components.

Here's a screencast!

[jbarchuk]

While watching your screencast I noticed two points that don't seen directly related but may point to a commonality that affects several bugs and may be of interest to the developers.

Odd #1.You first placed the hole into the top plate, and that went through both plates. You referenced the position at 20mm from the front of the top plate. Later after some different edits that reference seemed to have -transferred- itself to the -bottom- plate.

Odd #2. When you originally placed the pattern of 3x3 holes they appeared to go through both plates, but when you pressed the okee dokee button the new holes -disappeared- from to -top- plate yet they still appeared in the -bottom- plate.

So, *two* oddities (bugs/whatever) that affected features that -started- in the -top- plate, and then mystically-magically moved to the bottom plate, that's not a coincidence that's a pattern. Both oddities together may help point to the source of the -one- bug that caused -both- errors.

My intuitive guess is that's it's a *typo* in a variable or other data structure definition that applies to 'one' object -vs- another data definition that applies to 'more than one' object.

[jeff_strater]

Regarding the original issues:

1. you can edit the references after adjusting the diameter, you have to just re-select the hole center manipulator:

once you are there, you can edit them by just selecting new edges.  Fusion will remove one of the other dimensions to prevent over-constraining the hole:

I agree that this is not discoverable, and we have been discussing this for a very long time, and haven't come up with a great way to make those references easily editable and still preserve a nice smooth workflow in the most common cases.  Today, you can select those references without having to go back to the dialog.  So, you can just pick the face and two edges.  We discussed putting selection items in the dialog for the edge references, but then you would have to go back to the dialog to enable those selections, so in a lot of cases, the workflow gets a bit more clumsy.

2. I was not able to reproduce the problem in your screencast where editing the hole feature shows the wrong references.  It certainly looks like a bug - if you happen to have the model around, attach it and we'll take a look.

3. I was able to reproduce the third issue.  I'll file that bug.  However, there is a way to get the pattern to work like you want.  It is a bit subtle.  In your screencast, you have "Pattern Faces" selected as the pattern type.  This should work, I believe.  But, what I think you really want is "Pattern Features".  Face patterns are an optimized pattern compute that just copy the selected faces around, then join them into the body.  It is fast, but sometimes behaves differently than might be expected.  Feature pattern actually reproduces the feature recipe for each instance.  I tried it in this case, and it worked OK:

   

Jeff Strater (Fusion development)

[TrippyLighting]

Hi Jeff,

you are correct that I can re-select the references by clicking on that center manipulator, but as you say it's not immediately obvious. As an alternate method clicking on the slection field in the dialog would be more obvoius.

I also tried to create that pattern using "Patern Featuers" as you suggested, but as can be seen in the screencast this did not work. If it worked for you, could you create a quick screencas showing what workflow you followed ?

Here is a screencast that shows the workflow to recreate the incorret hole location reference.

[TrippyLighting]

Here's yet another quick little screencast to show strange behavior whe attempting to edit the hole pattern that was reated in the last screencast.

I would have attached teh f3d file but the @#@(&$ web interface complains:

"The contents of this file doesn't match its file type"

Please provdie an email, so I can send it to you.

[113746]

Hi Trippy,

Please send your f3d to jeff.strater@autodesk.com and yanhua.li@autodesk.com. We will look into it asap.

Thanks,

Yanhua Li

Fusion 360 Quality Assurance

[Mike.Zhang]

Currently it’s a limitation in Fusion 360, there should be a task to make this workflow more smooth.

We’ll work on it to make it better in future.

Below is a workaround to make it for now:

1. Create the two models as Bodies before turned them to Components.
2. Add one Hole through them.
3. Add the Pattern base on the Hole to get what you want.
4. Use Create Components from Bodies to get two components.
5. Final result.

 

Hope this simple introduction helps.

[Mike.Zhang · Accepted solution]

We've logged one issue to track it.

FUS-15859

Thanks for your information.

[TrippyLighting]

Hi Mike,

I call this a bug, not just a limitation as I cannot do what I should be possible to by all means.

The workaround as has several unwanted consequences:

1. Bodies cannot be joined, or grounded, that only works on components, so the joint can only be created AFTER I have created the hole.
2. That means, when I change the offset using the joint, the holes will not align anymore between the top and the bottom plate.
3. if I created the bodies using a sketch and later on want to export the part for reuse in another project, I lose the sketch as there is another bug that prevents me from moving a referenced sketch into a component, even if it is only referenced by that component.

This Idea in the Idea Station has already been accepted to be in the next release ad it only makes sense if this bug is fixed.

Expecting that this will be fixed, however, I accept this as a solution.

[O.Tan]

I guess I should also make a note that in a situation where I have the hole cutting through 2 components. The first component where I first placed the hole will have the usual hole properties (able to resize and etc) but the hole feature on the 2nd component will be sort of broken as in I wont be able to edit the hole (resize or re-reference it)

[Mike.Zhang]

Yes, we also can treat it as defect.

Thanks you.

[Mike.Zhang]

The 2nd Hole will be editable too. This issue is focus on the Pattern on the Hole which through two components.