topic Re: Inventor Bolt List in Inventor Forum

Inventor Bolt List

FORBESWILSON6174 — Sat, 28 May 2022 11:50:14 GMT

Further to a previous post on Bolt Grades, I am not winning in creating Bolt Lists in Inventor.

I know Inventor will populate a Parts List with the Bolts in an Assembly, however that is not ideal as it messes up the column widths and format of our Parts List.

Is there a way to create and populate a Custom Bolt List that can be inserted into an Assembly drawing and be exported to excel to provide a Supplier.

We have managed to export Bolted connection parts inserted from the Content Center, but the we can't do anything with the connections created from the Design Bolted Connection.

We can obviously export the list to excel re-name it and modify it, but how can we import the list back into the Inventor drawing.

With all the users out there, I am sure someone has figured out a way to create a Bolt list from an Assembly.

Any help / suggestions will be greatly appreciated.

Regards,

Re: Inventor Bolt List

A.Acheson — Sat, 28 May 2022 17:13:31 GMT

This isn't an easy task an the outcome will vary based on how the data is all ready set up.

Your looking for the fasteners only to be displayed in a parts list in the drawing. This is likely the most difficult way to display the information. The reason being is the interconnections between the partslist structures, balloons etc. Generally there should be only one parts list per assembly and the structures( structured, parts only) are fixed after initial ballooning and parts list creation. There might be workarounds of having separate drawings etc.

Questions:

How are you currently identifying a part as a fastener? Have you an item category or some identifier set up?
Are you using CC parts out of the box are have you modified the library with custom columns etc?
Are you trying to balloon the list of fasteners afterwards or is it purely for purchasing needs?
Is the fasteners list present on the drawing entirely necessary?
Can you provide images of the finished information how it is currently displayed and the issues this brings?

What can be done:

I would suggest splitting the data from the Assembly BOM rather than the partslist using ilogic and then send to either an excel spread sheet or to a custom table on a drawing. Otherwise a manual approach will involve multiple steps and a frustrated user.

Re: Inventor Bolt List

cadman777 — Sun, 29 May 2022 15:48:12 GMT

You may not want to hear this, but I NEVER use BoltedConnections b/c it has too many problems.

Apparently those problems have not been fixed for over a decade!

Instead, I make a fastener group (a bolt assembly) and label it with a custom MARK number.

Then to at the end of a project, I make a separate drawing (or drawings) that calls out only fasteners.

On that drawing I make a custom PartsList that will show only fasteners.

I use only 2 kinds of fasteners:

1. Assembly (any combination of bolt, washer, nut, etc.)

2. Part (any individual fastener, such as a bolt, or a nut, or a washer, etc.)

That's the easiest and most simple out-of-the-box way I found to make a fasteners drawing that is easy to read and follow.

The way I make sure the correct data is automatically inside the fastener assembly is to Link the individual bolt's Parameters to the Assembly Parameters. Then I use those Parameters in the Assembly file's Name/Description. So for example, each bolt has a 'GD' for diameter, 'NLG' for length, 'TPU' for thread pitch, etc. The Name/Description would be something like this: "=<GD>-<TPU> x <NLG> Long". The part's Parameter values would show up in the Assembly's Name/Description, which in turn would be a column in the BOM and PartsList.

Whenever I need a different size, I just copy the fastener assembly to a different file name, swap out the individual bolt/washer/nut, and update the Assembly Parameters dialogue with the new bolt's Parameters (have to delete the existing Linked Parameters first). This can be automated using iLogic if you do it a lot.

All holes are done inside each individual part. So the other job is placing all the fasteners. That could be time expensive in big jobs. But I've not found a more reliable way to do bolting on structural and machinery projects.

Re: Inventor Bolt List

pcrawley — Sun, 29 May 2022 23:57:00 GMT

Can you use the Parts List filter to achieve what you are looking for?

You said the standard parts list from the assembly "is not ideal as it messes up the column widths and format of our Parts List" - but this filter removes (or shows) standard content. So you can remove Standard Content from regular parts lists, and show it on separate/different-style bolted connection parts lists.

Like you, I'm no fan of exporting BOM data and manipulating it because the link to the model is broken - and that always ends in errors.

Re: Inventor Bolt List

FORBESWILSON6174 — Mon, 30 May 2022 06:37:09 GMT

Thanks for the reply, I appreciate the feedback. We are looking for the best option, and tried B/C as it gives you a complete bolted assembly as opposed to parts inserted from CC. We were not aware of problems with it, so thanks for the feedback.

B/C did give us problems in extracting the information from the Rule our engineer wrote, so it may be the best option to can the B/C.

Creating connections from CC is also not really an option as it does not give you a bolted assembly, and too many Parts.

That then leads us to the option you have mentioned. I am interested to know more about the Fastener Groups you create, and more about how you manage the different diameters, lengths and bolt grouping.

Do you have a single bolt assembly and pattern it as required?

The model I have just done has over 1400 Parts / Assemblies with a fair number of different lengths and Bolt groupings, so I need to be clear on how to deal with that.

I would appreciate more feedback.

Re: Inventor Bolt List

FORBESWILSON6174 — Mon, 30 May 2022 06:38:09 GMT

Thank you, I appreciate the feedback, I will give it a go.

Re: Inventor Bolt List

Frederick_Law — Mon, 30 May 2022 13:00:32 GMT

You can copy any part in CC to a new Library and change it there.

I copied and make my own A352 bolts.

Also another set of CSA structure.

Re: Inventor Bolt List

cadman777 — Mon, 30 May 2022 21:08:18 GMT

Thanx for the info and visual.

I've done similar (see below).

The problem with doing structural in Inventor is connections.

It's always been a problem, and I haven't yet found a good work-around for it.

So using my method effectively depends on how you put holes in your connections.

I put all the holes in the individual parts.

I never put holes in the assembly.

The reason is b/c it's way too much work to chase around the holes when the model changes, to make sure they all updated and are accurate. So I do everything with one master file that has various wireframe sketches, and Derive the relevant sketches into the individual part to make that part. Then all the parts (or most of them) are Grounded at the Origin, not using any Contraints. That cuts way down on computing overhead.

The thing that makes this work is how I setup the FamilyTable in the CC for all fasteners. I did a major update on all CC parts so they all have the same iProperties. That way, when they are part of the BOM/PartsList, there's minimal fiddling around with the data. Pretty much every data field populates the way it should b/c of how my CC is setup.

I usually do all bolting last using a combination of 2d and 3d sketches to place points relative to existing sketch geometry. Then I go to the connecting parts (plates, beam flanges and webs, etc.) and add the holes. Only after that do I add the bolts in the assembly. It's NOT automatic like BC, but it's accurate and reliable.

You can make the bolts adaptive so the washer/nut combo slide along the threads so when you place it you don't have to worry about whether or not the bolt is contacting the members. Most of the time most of my connections are standard (such as 3/8 plate for all railing clips), so the bolt lengths don't vary that much.

Anyway, find attached an example of how I make a fastener assembly. In the PartsList I call the fastener assembly a 'Fastener Group' (FG), and individual fasteners are called out by name. For example: hex nut (HN), flat washer (FW), taper washer (TW), hex bolt (HB), etc. I'm betting you can easily automate assembling these FG's using iLogic. You may even be able to size them and place them in your assembly using iLogic. But I'm no expert in iLogic, so can't be sure.

Back in the early 2000's when I began using Inventor to do structural work, the engineering firms were amazed that all the bolt holes lined up in the field, and 'no bolt was left behind'.

Re: Inventor Bolt List

A.Acheson — Tue, 31 May 2022 13:51:10 GMT

Do you currently have fasteners in your current model? Can you show the browser tree or the raw data you are working with and how they are currently set up? From what I read it really is just a data management issue. Whatever method you choose to contain the data you still need a way to separate the parts from the fasteners. Using standard content won't work cleanly as you likely have used a lot of CC parts. You will need a custom iproperty in CC called say Fastener or if you use part numbers maybe there is a pattern to follow to filter the fasteners. Then you can filter either manually or by code on this.

Re: Inventor Bolt List

FORBESWILSON6174 — Tue, 31 May 2022 06:29:46 GMT

Thanks for the feedback, this we have done, but it is a work in progress exercise.

Re: Inventor Bolt List

FORBESWILSON6174 — Tue, 31 May 2022 10:10:25 GMT

Thanks for the files and the info.

Like you, I also started using Inventor in the early 2000’s, and I also use one master file and derive my parts from it, I also put all my holes in the Single Parts.

I moved on to Tekla in 2007, but continued to use Inventor for Parametric Chute work, and recently I have been working with a company that is using Inventor for Structural and Mechanical Projects, hence the need to create an effective Bolting and Listing system.

I created a Custom Content Center folder and created a custom bolt as a test, but still a lot of work to do there, which is why I am trying to find out as much as I can about it.

Making Bolts adaptive is essential, (not sure how to do this), however there are things that I don’t understand.

Your comment on doing the Bolting last, I agree with, but I am not clear on the 2D and 3D sketches.
Why are they necessary if you create the holes with the Part?
Do you Pattern your Bolt Assemblies?
Do you have a separate assembly for each bolt diameter, or how does your Library work?
How do you deal with the Assembly mark when you change length etc.?
Where did the Part Numbers come from in your BOM?

Once we come to terms with what needs to be done, I am sure the engineer I work with will be able to use iLogic to assist in the process.

Re: Inventor Bolt List

FORBESWILSON6174 — Tue, 31 May 2022 10:38:15 GMT

Thanks for the feedback.

Initially I started showing bolts in the model, a combination of items placed from CC to create a bolted connection, and of bolted connections from the Design / Bolted Connection, but we ran into three problems.

The parts placed from CC listed ad individual parts not as a bolt assembly in the Parts List.
The bolted assemblies are created in separate folders and we could not extract the information using code.
The presentation on the Parts list is not the same for CC items and BC items.

For this reason, I have only shown a few connections, and we have not listed the bolts.

We know we can create custom properties for Fasteners which can be read, but not in BC because we cannot access the data from what our engineer tells me.

The BC fasteners would be far quicker to use, however if there are problems with software it is pointless pursuing this option.

Once we can capture the data, I think the rest is relatively straight forward.

Bear in mind that we are setting up a new system here for future projects, so everything is still flexible.

We are looking for the best and quickest option available.

Re: Inventor Bolt List

cadman777 — Tue, 31 May 2022 11:15:43 GMT

I do what Alan says by using a User CC fastener Family.

That necessitates saving the out-of-the-box CC Family as a User Family so it can be edited.

Then you can do whatever you want.

I created an iProperty for all CC parts called SIZE.

That's how I filter parts in a 'Summary BOM'.

There was a guy in here that did what you're doing.

His company created their own 'simplified' fasteners and structural shapes.

That way they could make large structures with much less computing overhead.

They also used a combination of iLogic/VBA and structural weldments to modularize their connections.

So you can start from scratch and create two libraries if you want.

One would be all fasteners and the other would be connections and miscellaneous structural elements.

It's a lotta upfront work, but it appeared to work well for them.

In order to accomplish all of this, you need to be able to do 3 things:

1. Create from scratch (a LOT of work!) or modify a CC library,

2. Write iLogic/VBA code, and

3. Setup a standardized connections library.

Lotta work!

If I was doing structural work all the time, I would quit using Inventor for it and go to something like Parabuild, or if you can afford it, Tekla Structures. All the CNC mills use Tekla data.

Re: Inventor Bolt List

FORBESWILSON6174 — Tue, 31 May 2022 13:41:01 GMT

I understand the necessity of creating a User Family, that I don’t have a problem with.

As I understand it, we still need bolted assemblies similar to those you have created, yes / no?

They will all have to have assembly and part numbers and iProperties etc., what I am not understanding is this :-

In your Assembly model when you want to create a bolted connection, you have to place Assembly ‘X’ from your CC into the model, which reflects Assembly X in the browser.
How do you add / adapt your Assembly to cater for different Lengths, because the Assembly number would have to change owing to a ‘new’ part.

Once we understand the method you are using, we can set up a system, and once it is working, see if we can improve on the methodology.

The engineer I am working with on this, can write iLogic/VBA code so I am sure he can come up with something.

I don’t particularly want to get involved in a standard connection library, it would get too complicated, and I agree with you that if you want to do Structural Detailing an a larger scale use the software designed for it.

Tekla is a great detailing package, but has become too expensive to maintain and unless you are tied in with a workshop with a lot of work I don’t believe it is worth it. Advance Steel is an affordable option and interfaces well with Inventor.

Re: Inventor Bolt List

cadman777 — Wed, 01 Jun 2022 01:59:24 GMT

Thanx for the additional info.

Let me answer your last comment first:

Yes, Tekla is for those with deep pockets.

Can't comment on AS, but can comment on Parabuild.

From past research, I hear that AS does NOT interface well with Inventor.

You need to use NavisWorks (or one of the Navis apps) to get AS to work together with Inventor.

Also, Parabuild has a very reasonable price-point compared to AS.

Disclaimer: I do not advertise for Parabuild, nor do I get any kick-backs from them. I just like how easy and simple it is to use and how much can be done with it.

Disclaimer #2: I would not use a structural program to do Architectural miscellaneous steel, nor most custom miscellaneous steel. That's what I use Inventor to do, b/c there are too many exceptions and options that I always run into when doing that kind of work, which the structural software doesn't have the capability to achieve without jumping through hoops. And that included Tekla Structures. What a PITA Tekla was for making stairs and railings!

Note: You're not placing assembly (iam) 'X' from the CC.

You manually made that and it's in a library, or you copy it from one of your previous projects.

But 'yes', you would still need some kind of bolted assembly.

You can make your bolted assembly using:

1. an iAssembly (I wouldn't waste my time w/this method, way too much overhead and problems), or

2. CC parts assembled (iam) manually or by using iLogic/VBA/VB.Net, or

3. a simplified part (ipt) that's created using iLogic (turn on and off features, drive the sizing with an excel file or Multi-Value Parameters, etc.

You can name the file like the structural programs do using codes to identify the parts of the fastener assembly (sort of like I do, but simpler).

I manually change the size and length of the fastener assembly when I need a new one.

Usually I 'steal' one from a previous project, and then swap out the parts to the correct size and length.

Then I delete all the old bolt iProperties and reLink them to the new bolt so they show up in the BOM/PartsList.

So for the fastener assembly I sent you, if it needs to change from 1/2 to 3/4, I would:

1. save the assembly as a new file with the correct size designation in the filename, then

2. RMB on each part in the assembly and pick the correct size from the CC, then

3. go to the Parameters DB and delete the Link to the bolt part. Those Parameters (GD, NLG, TPU) will then become User parameters, which I rename by adding a '0' at the end to differentiate them from the Parameters I'm going to Link to. Then Link to the same parameter names in the new bolt part (the one you just replaced). And then replace the old Linked Parameters in the value fields of G_D, G_L & THD with the same Parameters you just Linked to (I do this by deleting the '0' off the parameters in the value field). And then delete the 3 old Parameters.

The key here is saving all these assemblies and parts either in a User repository (on a local or network drive) or in the ProjectFolder. I usually create a directory named 'Fasteners' in the local Project folder, and drop all the fasteners and fastener groups into it so I always know where to find them. In other words, I DO NOT CREATE OR USE Inventor out-of-the-box library parts that are created and saved in the Inventor CC Library folder. If you want to save your Custom CC parts in that folder, then that's up to you. But I found that if the fasteners reside in the local Project folder, then if IT or some other idiot disconnects or deletes the Inventor out-of-the-box CC Library folder from your computer (or the network drive!), then you don't lose any of those fasteners, and your project won't be broken (missing parts) when you go to reopen it or reuse it in the future. Talk about a mega time killer! 'Once burnt, twice shy.'

Here's an explanation of the method used for lengthening a fastener group but not changing the diameter:

1. Save the assembly under a new name

2. Since the bolt is the same size, the washers and nut won't need to be changed, so forget about them

3. RMB on the bolt and change the size.

4. Check your Constraints to ensure the GRIP is correct.

5. Then place that fastener into the assembly wherever needed.

Your engineer may even be able to automate sizing and placement of the fasteners based on the hole size and thickness (GRIP) via 3 user inputs/picks of the mouse. It would be awesome if he could do that! If I could CODE, I would have done it a long long time ago. 😐

And if you have 3 fastener groups with the same length bolt and same number of washers and nuts but different GRIPs, then you can group them all together in your BOM. The BOM becomes easy when things are simple and uniform. You just need to come up with an iProperty or iProperties that'll cover all the bases so you can group all fasteners of the same type.

Re: Inventor Bolt List

A.Acheson — Wed, 01 Jun 2022 04:28:16 GMT

Here is one option with the minimal adjustment of standard content.

Requirements:

Create a custom Library for the fasteners in CC and add an iProperty "Fastener" and link to Category> Change as needed
Create a new parts list style name it Fasteners and give it a title "FASTENERS" and add a column with iproperty "Category"
To your standard Partslist Style add a column with iproperty "Category" set width to 1mm to avoid it being shown
Add two partslist to the drawing. One Standard style and one Fasteners style.
Run the external rule this will turn off Fasteners rows in the Standard partslist and do the opposite in the Fasteners partslist.
Export to excel the Fasteners partslist manually or add to the ilogic code and export by code.

The item numbering might get a bit out of sync but that can be looked at as a separate side defect.

'  a reference to the drawing document.
    ' This assumes a drawing document is active.
    Dim oDrawDoc As DrawingDocument
     oDrawDoc = ThisApplication.ActiveDocument
   
    ' This assumes that a parts list is on the active sheet.
	oSheet = oDrawDoc.ActiveSheet
	'Loop through all sheets if partslist location is unknown
	'For Each oSheet As Sheet In oDrawDoc.Sheets
		 '  a reference to the parts list on the active sheet.
		For Each oPartList As PartsList In oSheet.PartsLists
			Dim i As Integer
			Dim oRow As PartsListRow
			If oPartList.Title = "FASTENERS" Then
				'[Working with the contents of the Fasteners Partslist
			    For i = 1 To oPartList.PartsListRows.Count
					' Get the current row.
					oRow = oPartList.PartsListRows.Item(i)
					oCell = oRow.Item("Category")
					If Not oCell.Value = "Fastener" Then
						 oRow.Visible = False
					Else
						oRow .Visible = True
					End If
			    Next
				'] 
			Else
				'[Working with the contents of the main partslists(Need to exclude Fasteners)
			    For i = 1 To oPartList.PartsListRows.Count
					' Get the current row.
					oRow = oPartList.PartsListRows.Item(i)
					oCell = oRow.Item("Category")
					If oCell.Value = "Fastener" Then
						 oRow.Visible = False
					 End If
			    Next
				'] 
			End If
		Next
		'Next

Re: Inventor Bolt List

FORBESWILSON6174 — Wed, 01 Jun 2022 07:00:05 GMT

Thanks for the feedback, I’m getting somewhere now.

I realise that the Bolted assembly is a ‘Library’ item

Looking at both your and Alan’s response, you use the CC and don’t create a Custom CC, but if you are using a custom folder for Fasteners it may not be necessary to create a CCC.

So for marginal grip length changes in the Assembly that don’t affect the Bolt length, the Assembly will show a clash?

Thanks, I will work through all this info and see if I can get this working before moving on.

Regards,

Forbes

Re: Inventor Bolt List

FORBESWILSON6174 — Wed, 01 Jun 2022 07:00:34 GMT

Thanks for the feedback, it could be very useful.

I will work through all this info and see if I can get this working and if we can include it into the iLogic we have for the rest of the mode.

Regards,

Forbes

Re: Inventor Bolt List

cadman777 — Wed, 01 Jun 2022 13:05:11 GMT

So for marginal grip length changes in the Assembly that don’t affect the Bolt length, the Assembly will show a clash?

In that case, you would have more than one assembly of the same components, unless you use Adaptivity or Flexible assemblies (probably be way too much computing overhead for this method). Even if the filenames and grip lengths are different, if the filtering iProperty/iProperties is/are the same for all of them (including your MARK # being the same), and your filter uses just the iProperty/s to merge the occurrences in the assembly to tally-up the total quantity, then NO, it won't be affected.

If using CC parts in an assembly (iam), there will be no weight difference.

If using a simplified part (ipt), there will be no weight difference.

The weight difference is the indicator I use most of the time when the parts are the same length but may have different end conditions or holes in one and not the other.

Re: Inventor Bolt List

FORBESWILSON6174 — Mon, 13 Jun 2022 16:01:48 GMT

Having now gone a bit further with the whole process, the Filter option would be perfect if I could change the Part designation to 'Bought out' items.

I looked through the posts, and found a thread from 2013 asking the same question, but I never got an answer.

Hopefully after 9 years it can now be done.

You can see from the Filter that the Custom bolts are regarded as parts and won't filter.

If I can get an answer to that, it will solve that problem.

Regards,