More efficient way to place bolts within an assembly?

[Anonymous]

My team and I are new to using Inventor and have just completed our first full assembly. We work on substation design and during the assembly process we found it extremely tedious to insert hundreds of bolts in order to constrain the model as a whole. I am curious if there is any automated feature in which the software can detect holes of a certain size and intuitively place and constrain the necessary bolts all at once?

[SharkDesign]

You can turn on autodrop when you place a bolt/washer. It will find every hole of the same size in that face and drop multiple bolts. 

There's also the pattern function when you insert the bolt. If you've used a pattern to create the holes it'll put a bolt in all the holes of that pattern.

[swalton]

It depends on how you build your models...

The Bolted Connection Generator tool in the assembly environment can help.  I don't bother with it because it requires using Content Center fasteners, which we decided not to use 12-15 years ago.  I'm also very interested in how that tool effects regeneration time on large assemblies (think 1-2k fasteners per top-level-assembly).

I use a combination of feature patterns in my base parts and component patterns in my assemblies.  The part-level feature patterns serve as the seed of the assembly-level bolt patterns.

The basic workflow is like this:

1. Create the base part, like a rectangular foot plate for a column.
2. Add a single hole in one corner of the plate.
3. Use the Feature Pattern command to make a rectangular or circular pattern of the bolt hole.
4. Place the base part in an assembly.
5. Constrain, using the hole pattern, to the mating components
6. Add the bolt, nut and washers to the assembly.
7. Constrain the bolt and any washers to the seed hole on the foot plate.
8. Constrain the nut and any washers to the mating components.
9. Select the bolt, nut, and washers.
10. Start the component pattern tool
11. Select the feature pattern in the foot plate.
12. Hit ok.
13. Inventor will populate all the patterned holes with the bolt, nut and washers.
14. Repeat for all other hole patterns in the assembly.

[Anonymous]

Something that jumps out to me: 

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insert hundreds of bolts in order to constrain the model as a whole.

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Are you constraining before placing the bolts or relying on the bolts to keep your model constrained? It may seem like semantics, but it is a key distinction. Constraints between components(not bolts) should be doing the heavy lifting and the bolts should be there for eye candy. Yes I know they are important for BOMs, weights, sizing, etc. but I'm sure you get my point.

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[cadman777]

When I read your inquiry, I flagged the same statement that ckurre mentioned.

My method is similar to swalton.

Let me add this not yet mentioned:

I make an assembly of the kind of bolt set needed (øhb#_hn, øhb#_fw_hn, etc.) and use it throughout the top level assembly where it fits. That reduces the number of parts in the top level assembly, as well as allows reuse of existing parts (subassemblies). Placing this way requires only one INSERT Constraint per bolt hole, then array as needed. The main difference between these bolt assemblies is bolt length (if the hole is the same ø and the thru thickness is different by more than 1/4"), and if the bolt diameter is different.

But the placement process is tedious and takes a long time at the end of the design process. If I keep a running record of holes, it's much easier. Otherwise, I have to manually look at every connection and thickness to decides ø + length + washers/nuts/etc. Then make assemblies out of all of them.

Someone long ago had an iLogic program that automatically populated fasteners of the same kind, but I can't recall who had it. Maybe on Autodesk's Inventor Store? https://apps.autodesk.com/INVNTOR/en/Home/Index

If I was better at iLogic, I would make a small Rule that works like the DesignAccelerator BoltedConnections (which I don't use b/c it has too many defects), except it would be much simpler and work on existing holes. I would expect this SHOULD BE part of Inventor already.

Incidentally, AutoDrop never worked for me, b/c it never picked the correct ø which forced me to do more mouse clicks to get one bolt assembly placed. My method of creating a bolt assembly on disk with iMates was as fast a solution as I could create.

[mcgyvr]

RIP KwikSert...  Hopefully someone will pick up the torch there.. 

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=7927536498261408960&appLang=en&os=Win32_64

Hands down as easy as Autodesk should have made it work out of the box.. 

[cadman777]

That's what I mean by a simple pick-and-place rule.

Only thing is, someone else had one too, some guy from England, but can't recall.

He also had a very slick way of making automatic drawings in Inventor-AutoCAD...

[Anonymous]

I understand what you are saying and do constrain all other necessary elements of the assembly before placing the bolts, but still must use an insert constraint with each individual bolt which is extremely time consuming with the sheer number that must be placed. 

[mcgyvr · Accepted solution]

'..edit.. nevermind.. Holiday brain.. 

[Frederick_Law]

If you pattern the holes when possible, you'll save some time.

Mate one and you can use hole pattern to fill the rest.

[dg2405]

You can also use that iLogic-code on message 18:

https://forums.autodesk.com/t5/inventor-customization/rivet-assembly/td-p/6286291