Inventor Bolt List

[FORBESWILSON6174]

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,

[FORBESWILSON6174]

Moving along, I created new bolt parts using CC dimensions and populated it with the attributes I needed for my Bolt list. As you can see from the reply above it populates the Bolt list, but I need to be able to Filter out the bolts from the parts.

Still some work to do, but seem to be getting there.

Thanks to all those who replied, I will keep you updated.

 

[FORBESWILSON6174]

I created new bolt parts using CC data and added the properties I wanted, and it populated the list no problem.

As can be seen from the above reply, I need to be able to filter the bolts out of he parts list.

Still some way to go, but getting there, we will have to see what we can add code for, but that is for the clever people.

 

[cadman777]

Is this what you're referring to?

If you set all your fastener CC parts to 'Purchased', then you have it already done for you before you place a fastener.

Or do you mean that you want to use iLogic/VBA to set all parts to 'Purchased' and then to BOM>Filter them all as 'Purchased'?

[FORBESWILSON6174]

None of my parts relate to CC outside of the info extracted from CC.

Where do you set the parts to purchased so the BOB will recognize it, I couldn't find it.

[cadman777]

Lookin' good!

As was stated by others, you can add a column ('Purchased') to your PartsList, make it 1mm wide so it won't appear in the drawing PartsList, and use that 'invisible' column to Filter the PartsList the way you want.

[cadman777]

In the BOM editor, add the column ChooseColumns>Customization>BOM_Structure.

Then triple-click on it to select 'Purchased'.

Only caveat is, if you want your bolt assembly to be 'Inseparable', so that the individual parts don't show up in the BOM, then you will lose it if you want to use 'Purchased'.

I don't recall how to save all the fasteners as 'Purchased' in the CC (setting that iProperty). But if I was to guess, I would OpenFromCC a part representing the whole FamilyTable, then put it into a blank assembly, then change it in the BOM editor, then Save the part, then ReplaceFamilyTemplate in the CC_Editor. That probably will do it for you.

[FORBESWILSON6174]

You got it, I created a dummy assembly, placed a part in it and opened the BOM, tripple clicked on BOM Structure and changed it to Purchased.

If I do the same in an assembly, it updates the Single Parts as well.

Now to work on the Filters.

[FORBESWILSON6174]

Bingo, it works.

 Before Filtering

 

 After Filtering.

Now for Numbering and Testing.

I will leave the Post open for now in case I have other queries.

Thanks Guys.

Regards,

[cadman777]

Nice! Glad it worked for you.

[rhasell]

Hi

I might be late to the party, but I have an external folder with Master bolted assemblies.

I then use iLogic to build the bolted assembly and save it to the content center library folder.

If you combine this with iMates, working with bolted connections becomes a breeze.

[FORBESWILSON6174]

Thanks for the reply, you're not late, just in time.

What you are doing sounds like it will save us a lot of time.

I have got the custom parts to work, but I would prefer to use CC, but up until now we have not been able to extract the info to our Doc Control sheet, but that was mainly because we were using Bolted connections and we couldn't access the folders.

I am having a meeting just now with our engineer and I am sure he will be very interested in what you have done, as he can sort all that out.

I will give feedback after I have spoken to him.

Regards,

[FORBESWILSON6174]

Nicely set up, metric is always easier to deal with than imperial.

Your Libraries look like you have similar Assemblies with mm variations in length, is that correct.

We know that there is a ‘Grip’ range for each Bolt length assembly, and it would be nice to be able to drive the various grip lengths within that range using one assembly, after all, the bolt length is what you ultimately want.

You would certainly save a lot of Assemblies in the Library. This question of one length arose in an earlier reply.

I did pose the question on the Forum regarding Constraint Limits, however the response was that Inventor could only handle a minimal amount of Limits, so it bombed my idea out of having a ‘Floating’ Nut and Washer.

Could the limits be built in with iLogic using the CC Table ‘Grip’?

Regards,

[cadman777]

Not to cut into this communication, but that's what I was talking about above.

You have an iLogic rule picking parts out of your CC based on user input (hole size, near surface and far surface for grip, number of washers and type, same with nuts).

The rule can drive the length of the bolt based on the grip, washers and nut and the necessary extra length allowance (1/8"-1/2"  depending on the bolt diameter) past the nut.

The grip can be determined by the user input of picking faces (near side and far side).

You can use a mult-value parameter to drive the grip length min/max for each CC bolt length, setup in your CC part template.

So the user would pick a hole and grip, specify (radio boxes) washer type and number + nut type, then the rule would find the appropriate bolt length to satisfy that grip.

Then the rule would assemble the parts with the proper grip and then save it to the local or designated folder under a name commensurate with the assembly.

The only caveat is you would need to save the same bolt assembly with different grips under a different name, but have the same designation in the BOM so it will 'roll up'.

[rhasell]

Hi

Yes, I have heaps of assemblies, every time I need a new grip length, I make a new assembly.

The fasteners are custom content center library, using the copy to new library in the  Content center, these have a few custom properties for my own BOM needs.

The Length, for default parts list style,

Stock num and desc for my own uses, as I don't use the default.

TYPE to assist with BOM sorting (All bolts sorted together)

Mark to assist with BOM sorting (the 'z' places all fasteners at the end of the parts list)

Drawing note, some clients ask for a leader showing the bolt locations and length on their drawings.

My iLogic code is not fancy, the grip length drives an insert constraint.

The bolt length option is a guide, I still have to click on the bolt and select "Change size" The bolt length is based of the thread pitch, allowing a minimum of 1.5 threads past the nut.

So length is created from, add washer add nut, calculate the threads required based of the pitch, then estimate a minimum length. I then have to choose the closest bolt from the library.

The file is then saved to the content center and can be used in future builds. (also saved with iLogic)

Metric is king, it just makes sense, the banana scale is confusing.

[rhasell]

Parameters of a M16 Gr8.8, single washer bolt assembly

[FORBESWILSON6174]

You're not cutting into the conversation, the more feedback we have the better,

[FORBESWILSON6174]

Thanks for the feedback, I was hoping that somehow I could do away with masses of assemblies for each bolt length.

It seems that this is not possible, so the best option is to create a Library of the different option grip lengths 1/32" or 1mm increments for each bolt length and then use iLogic to select the bolt length from the grip as you are doing, or do what Chris does and place the bolt and accept the clash.

[johan.degreef]

Our solution is neither from perfect, but as the built in bolt connection solution slows the assembly down, we created simple CC part that contains the bolt, nut and washer. Disadvantage: they also appear in 1 line in the partlist.

[FORBESWILSON6174]

Thanks, if you are referring to the Design Bolted Connection, we can't use it for reasons stated in a reply above.

[FORBESWILSON6174]

I agree with you that some clients want bolt locations, so I added a column ASSY No. which is the assembly drawing number where the bolt assemblies are located.

The problem I am having is that the Assembly drawing number is the Model parameter PART NUMBER, and if I include

the parameter from the column chooser, it reflects the part number of the fastener parts.

Is there a way to get around this, as it does mean that you can create a GA which would list the bolts and the assemblies they are on.