Bolted Connection auto solve not working - Inventor 2026

[smctavishM7GRT]

I have a structural assembly with many bolted connections using frame generator. I noticed that a number of the bolted connections have bolts that are way too long (7" long compared to 1.75"). Switching the bolted connections to auto-solve (whether manually or using ilogic script) does nothing. The only way I can see to update them is to right click each bolted connection => select 'edit using design accelerator' then click 'ok'. Not sure why this is happening. Opening design accelerator and clicking ok is tedious (can take around 15 seconds per connection).

This post has been edited due to: @heather_tracy added the product to the title to help more community members find this topic. 

[CGBenner]

@smctavishM7GRT 

Hello, welcome to the forum!  Can you tell us what version of Inventor you are working with?  

For these bolted connections, did you use the same workflow to install all of them, and can you describe what workflow you used?  Maybe share some screen shots or a recording?  The reason I ask is that there is probably a clue why some of these are too long, and not all of them.  Thanks!

[smctavishM7GRT]

Using Version 2026.

The workflow to create them was using the bolted connection feature, I used the concentric circles create the bolted connections. I believe that these connection extended the bolt length due to changes in the frame. The frame was created using the frame generator, but angle iron clips were added to the assembly as separate parts. The issue isn’t so much that the bolts got messed up, its more that I can’t find an effective way to update. Opening each connection in design accelerator is tedious and time consuming.

[jyager]

That bolted connection tool is temperamental. Always has been. The auto-solve has given me problems before and I've had to go through and manual update connections like that. It's amusing that it decides for itself to update things to make them incorrect, but cant take it upon itself to fix them again.

[smctavishM7GRT]

The workflow to create them was using the bolted connection feature, I used the concentric circles create the bolted connections. I believe that these connection extended the bolt length due to changes in the frame. The frame was created using the frame generator, but angle iron clips were added to the assembly as separate parts. The issue isn't so much that the bolts got messed up, its more that I can't find an effective way to update. Opening each connection in design accelerator is tedious and time consuming.

[cid:[email protected]]

[johnsonshiue]

Hi! Please share the files that exhibit the behavior. I would like to understand the Bolted Connection issue better.

Many thanks!

[benY56W2]

I am also having this issue. I am using build 398 2026.3 Date 04/13/2026 on a windows 11 pro version 10.0.26200 Build 26200.

My problem is similar, but not quite the same. Instead of my bolts being too long, in my case the auto generated holes don't align with the rest of the auto generated hardware. It seems to be the only option is to left select and right click each problem bolt individually (in the model space or the feature tree - I cannot multiple select from either because then it doesn't give the 'edit from design accelerator' option) , choose 'edit with design accelerator', -*change nothing*- , and then just click OK for the software to re-align the hole with the rest of the generated hardware (bolt, washer, hole, washer, nut). Another nuance for my issue is that I am using these bolts in a master assembly, and these bolts are connecting a base plate of one frame generator subassembly to the column of a different frame generator subassembly, as it would happen in the field environment. 

As the OP said, this takes 12-15 seconds per correction when in reality it shouldn't be a problem in the first place.

Has there been any progress on this issue?

As an aside to the image I attached: Why doesn't the section view (half) also slice the hardware?

[lauri_barnhart]

Welcome to the community, @benY56W2.

Hope you are well. Tagging in @johnsonshiue to see if additional information can be provided.

Thanks,

[johnsonshiue]

Hi! The issue is usually geometry-specific. Please share the files that exhibit the behavior here. I would like to understand the Bolted Connection issue better.

Many thanks!

[benY56W2]

Thanks for the interest.

At this point I have rectified all of the connections and none have the issue anymore. I only had three dozen or so - I cant imagine having to deal with this problem on a grand scale..

Additionally I am unable to share any files - this is related to company policy. 

I am not sure exactly what you mean when you say it is geometry related. There are only four inputs for the linear bolted connection dialog box (Start plane, Linear edge 1, Linear edge 2, and Termination), and as I mentioned -none of the user inputs changed- the fix involved simply opening the dialog box for each individual bolt and affirming the selections. This seemed to cause inventor to re-consider the placement of the corresponding hole for that bolt. I am not sure why this needed to be done independently when the whole model was regenerated after the two assemblies shifted in relation to each other. 

Ben

Edit: I threw together a project with a similar scenario that shows the problem ('26-0820 BC Test PnG.zip) attached.

This is a generic re-creation of my original problem - two frame generator assemblies mated inside a master assembly, attached to each other with a bolted connection. When one of the mates is adjusted (pesky customer requests) the holes do not seem to follow the hardware that they were created by, even after a rebuild. The bolt, washers, and nut all move as they should, but the holes do not seem to.

[johnsonshiue]

Hi! It seems to lack an update. When I right-clicked on the bolted connection -> Edit using Design Accelerator -> Ok, the hole did move to the right place.

Many thanks!

[benY56W2]

Yes, thank you - I thought I mentioned that in the previous dialogue. Either I have mis-spoke or I have mis-understood.

The bolt hole does not follow the hardware automatically - that is the problem. It should. 

I should not have to select each individual bolt and open a dialog box, change nothing, then confirm to force the update and cause the hole to reposition - it should reposition automatically when the assemblies change relation to each other.

I thought that being the problem was clear. 

How can I make inventor AUTOMATICALLY update the location of the hole when the assemblies move? This should not even be an option as I cannot think of a reason anyone would want to not have holes follow bolts properly.

This example has one bolt and hole. Please consider a person trying to model a large structure or something much more complicated with this software. 

[johnsonshiue]

Hi Ben,

Absolutely! The behavior exhibits in the assembly does not look right to me. Do you know how to reproduce it from scratch?

Many thanks!

[benY56W2]

Yes, I do. I attached a project that was built from scratch in an earlier post, and also described how I built the assembly in a post before that.

I am not understanding what I need to do to help convey this problem any clearer. 

[jnowel]

Just chiming in a bit on this.

I looked at your Test Pack and Go model,
It seems that Auto-Solve is NOT available when you have the "Enable sub-assembly Structure" is NOT selected

If you Right Click -> Component, "Automatic Solve" is  *NOT* present there

if the resulting bolted connection is created with a sub-assy structure, "Automatic Solve" option is present,

And there is a blue circular arrow symbol on the model tree (if auto-solve is enabled).

selecting "Manual Solve" removes that icon

[johnsonshiue]

Hi! The project team got back to me, confirming this was a limitation at the moment. As @jnowel correctly pointed out, when the BC structure is flat, the Auto Solve ability will be disabled. I am very sorry for not realizing the fact much sooner. Please feel free to submit an idea to Inventor Ideas forum, requesting this enhancement.

Many thanks!

[benY56W2]

Ah, thank you for this new information. I was unaware about the bolted connection subassembly structure option. I have been playing around with the PnG I made for this demonstration. It seems that the bolted connection must be created with this structure on or off originally - there is not an apparent way to convert a BC that was not generated this way originally. 

What has seemed to (mostly) solve the problem is just selecting the Manual solve option as you have indicated. It solves 2/3rds of the problem, because it updates the connection without having to open and click through a dialog box, and I seem to be able to select multiple bolts in the feature tree, RMB->Component->Manual solve and it will update everything selected. I am still slightly confused as to why this wouldn't be included inside a refresh subroutine deep in the code.

It is also a bit odd that in this selection menu there is a checkmark present (or lightening bolt indicating a needed update) as if this option is currently enabled next to the manual solve option, and regardless of how many times I select this option it will not clear the checkmark - it seems to be not un-selectable as a menu option, it seems to act more like a button hidden inside a drop down menu. It is interesting though because the problem occurs originally when the BC is generated (basis of my problem). If I click through and (try to) uncheck the 'manual solve' option, the problem disappears, but the manual solve checkmark doesn't change (as described above). If I repeat this process again, the problem returns.

It is as if the checkmark is stuck on, but the 'manual solve' option is in fact originally off (though shows as on), then gets actually turned on and fixes the problem in the second iteration of the test process, then gets turned back off in the third iteration of the test process(though still shows on) and the problem returns - all the while the checkmark for the manual solve option is present (showing on).

Not sure where to go from here, maybe someone can look into the code that shows that checkmark as displayed or not, it seems to be faulty and shows always on.

I can accept it as a work around as it seems to work in the large model I was working in when I discovered it. Checking the 'manual solve' option after selecting all the bolts that require the update starts an automatic string of processes that renders the computer and inventor un-useable and seems to take 2-3 times longer amount of time that individually opening each bolt and clicking through would - but it is done in the background meaning I can select all 200 something bolts and start the process, and then go to lunch or come back the next morning while the program crunches - somewhat of a workaround ...somewhat. In our field it is not uncommon to leave a computer crunching overnight to perform large pipe flow calculations, generate point clouds, or calculate FEA outcomes, I just didn't forsee it being necessary while updating bolted connections.🤷‍

Thank you all for your time and effort.

[jnowel]

The sub-assy structure was the "original" Bolt Connection feature (and maybe that's why it had the "full" functionality.)
The flat structure, I believe was introduced in the 202X version (I can't recall when exactly)

I don't use Bolt Connection much especially in a large assy so I don't have much experience finding the 'optimal' way.
But what I did in the past was also toggle on/off the "Automatic Solve" to update things (and seeing the icon on the model tree help confirm on my end the status).
I turn it off mainly because on the back of my head, I don't want Inventor to always solve and take 'unnecessary' compute time.

And also prevent potential 'random' crashes when it tries to auto-solve things. <-- this is mostly anecdotal and I just have this 'fear' that it may crash unexpectedly.

[benY56W2]

I have a similar fear - but it seems to be autocad/inventor based. I never noticed it when working with other programs like Solidworks.

My problem is that I need to cut holes into parts in the assembly environment, and it seems the only 'intelligent'

 way to do that is with bolted connections (and the holes that it generates)

Am I missing something? Hopefully?

[jnowel]

The steel frames I made are likely relatively small in terms of scale.
I am usually either using multibody/skeletal modelling when possible or FrameGenerator but I mainly keep track of the holes.

Sometimes even a mix of skeletal modelling then derived parameters (so I can "reuse" assy and the detail drawings with minimal changes).
Fasteners I put last and, in some projects, I did not even put them (and I just put in the general note the fastener type/configuration) that's why I don't have much experience in Bolt Connections.

Edit:
I found the Hole Projector addin useful as well in some of my projects.
There is some updated beta version found here: Solved: Re: Add-in repeatedly fails to load - Autodesk Community