Constraining patterned arcs and circles

[PremTM]

Hello.

I'm having an issue with a simple thing at first glance. Attatched below are 2 .ipt files containing only 1 sketch each. What I would like to do is to create a base consisting of 4 pillars connected by a piece sitting within boundries made of 80mm arcs tangent to those pillars (sketch in P_1.ipt is quite obvious).

The task should be extremely easy - draw a circle+dim constrain it -> rectangular pattern it. Draw an arc tangent to 2 closest circles -> circular pattern it. (Why not fillet the edges instead? Because pillars will be extruded higher and they're supposed to be easily adaptable - by changing sketch parameters rather than fillet radius. Also the result is 1 sketch less in the tree.)

The problem that arises - patterned arcs (or features in general) in sketch mode are missing coincident constraints, which results in them being not extrudable. In some cases running a sketch doctor might work, but not in this one. You can't pick any lines in order to close a loop and you can't add any more constraints because you'll overconstrain the sketch.

In P_2.ipt I've gotten rid of circular pattern for arcs, added 45deg sort of construction lines and closed the loop by adding small arcs, which fill in the gap between those 45 deg lines and big arcs. Now I can extrude it in a few ways but then I have to pattern the solid object. (I could also get rid of rectangular pattern for circles - just aknowledging that I know it's unneccessary at this point.)

It works but the issue with this approach is that this workaround is not "obvious", not as simple as it should be and not as clean. It adds another operation to the tree, where there would be none otherwise.

My questions are:

• Is there a way to add such constraints to make the P_1.ipt approach work?
• If not, is there any better way of handling such task than what I've come up with in P_2.ipt?
• How do you - experienced (power) users handle things like that?

.ipts were made with Inventor Professional 2019.

[JDMather]

See Attached.

[SBix26 · Accepted solution]

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@PremTM wrote:

.....

It works but the issue with this approach is that this workaround is not "obvious", not as simple as it should be and not as clean. It adds another operation to the tree, where there would be none otherwise.

My questions are:

• Is there a way to add such constraints to make the P_1.ipt approach work?
• If not, is there any better way of handling such task than what I've come up with in P_2.ipt?
• How do you - experienced (power) users handle things like that?

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Let's start by reversing a couple of assumptions:

1. Simple sketches are better modeling practice, usually one feature defined in a sketch

2. Patterning features is almost always better than patterning sketch elements

With that in mind, P_2 is the simpler and more obvious solution, to me.  I would, in addition, make the two circles and the 45° lines construction line types so the sketch geometry is even more "obvious".  You could even simplify the sketch further by making just half of what you have now, extrude it, mirror it and then circular pattern.  This makes three features where you now have one, but that's not a bad thing.  The bad thing is having busy, complex sketches.

In my attached file (Inventor 2019 format), I did what I described above, and all of the parameters (except extrude distances) are still contained in the first sketch.

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Sam B
Inventor Pro 2020.0 | Windows 7 SP1
LinkedIn

[PremTM]

Thank you for your reply!

I don't think you've hit the core of the problem here. I know Inventor sometimes has issues with picking the right geometry for extrude command. Why I was unable to pick any geometry was because of coincident constraints missing after sketch pattern application and my questions in general concern fixing issues which arise from using patterns in sketch mode.

You have created the same drawing without using pattern command, which I take as something like "You can't fix it easily, better draw and constrain each element individually to avoid issues in such scenarios". And it pretty much indirectly answers my main question. 😄 

[JDMather · Accepted solution]

In order of preference:

1. Pattern Bodies rather than Features.

2. Pattern Features rather than Sketch elements.

3. Pattern Sketch elements when 1 or 2 are not appropriate.

My guess is that the new Sketch Profile selection in 2020 would probably handle pattern sketch elements just fine (especially for this simple case) but the above rules are so ingrained into my modeling practice that I didn't even bother to try.

[PremTM]

Thank you for your reply!

With that in mind, P_2 is the simpler and more obvious solution, to me. 

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Sam B
Inventor Pro 2020.0 | Windows 7 SP1
LinkedIn

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Is it though? 😄 If I had to take a look at it first time and make changes to it I am pretty sure the sketch itself would not be anywhere near being "obvious" at first look. That of course changes when you take a look at the tree and see other operations.

However, your approach seems bulletproof and more efficient after all. Similar to JDMathers reply this indirectly settles the case of using patterns in sketch mode. Thank you for the tips!