Automating Dimensions in BOQ/BOM

[drawingsCHR7R]

Hi All,

I would like to automate the dimensions column in our BOQ, I have been able to do it for the mass, but I would now like to do it for the dimensions, I want it to show the 3 main dimensions, Width, thickness & length and depending if its a pipe or not then Diameter, wall THK & Length. I would like for this to update accordingly when I have made a change.

Is this possible?

Any assistance would be appreciated.

Thanks

[SharkDesign]

Do you use templates for this?

You can put your parameters into the iproperties and then show this in the BOM. 

So next to the parameters in the parameters window you'd click 'export' then in the iproperties...

say you wanted it in description, you write =size <L> x <w> x <hi> or whatever your parameters are called and it'd say something like size 20 x 30 x 5

This will update when the parameters change so you can just set it up as a template file with =size <L> x <w> x <hi> already in your iproperties and have a different one for pipes. 

Like this:

https://www.youtube.com/watch?v=aPn7QBzYzDg

[drawingsCHR7R]

Hi There,

Thanks for the reply!

Yes I have a template that I use and have some custom info set on.

I saw the video and how it was done but how would I do exactly that but with the "Dimension" column?

[drawingsCHR7R]

Maybe a bit more background on this, I have used a multi-solid body. The I used the make components command to put it into an assembly and now I would make a BOM based on the assembly, how would I automate the Dimensions column on the BOM using this workflow?

[SharkDesign]

That is more complicated, you can click 'include parameters' during the make components process, but you are driving it off your assembly. Your parameters all need to be unique, so for your first body in the multibody you'd use like hi1 w1 L1, then the next body you draw would be hi2 w2 l2 etc.

Then when you make components you'd do the above posted steps to add it to the iproperties. 

For editing iProperties on lots of parts from scratch (as you'd have to do with the 'make components,') the quickest way is to edit them directly in the BOM as shown below. You can also type the =<hi1> x <w1> in this way and it will populate. Remember that you need to click the export in the parameters window for each part (open each part and do this) as the export option tick is not carried through once you make components. 

There will also be ways to do this with iLogic which may be quicker. 

https://www.youtube.com/watch?v=pMo10YVvvV0

[drawingsCHR7R]

I have tried to do what you say but I don't think that I'm doing everything correctly. 

I have attached a multi-body solid, could you possibly show me on a screencast how you would do the automated dimensions?

Thanks

[SharkDesign]

Yes, will probably be tomorrow before I do it though

[drawingsCHR7R]

Understood. Thanks I will wait till then.

[SharkDesign]

This is how I was describing. (The end bit just shows how you can also do it from the BOM if you know the parameter names)

https://knowledge.autodesk.com/community/screencast/3fe037d2-6d41-4342-9dd0-aa5d6425b6c1

However, after seeing your model, you'd probably be better off modelling the curved section in sheet metal. 

You can still do it my way, or there is iLogic floating around that will get the dimensions of a flat pattern, but that's going to be even more complicated to set up.

[drawingsCHR7R]

Thanks a lot, I understand the workflow much better now and I believe this is ideal for smaller assemblies.

A few questions:
- Is there a way to streamline the the process of doing doing the dimensions as I have assemblies with much more parts, so it seems that the process of having to go through every part and do that typing will be just as time consuming as actually typing it out?

- Your dimensions went into the description column, I would like mine to appear in the DIMENSION column. How would I go about doing that?

Thanks for all the assistance!

[SharkDesign · Accepted solution]

If you are methodical about your parameter names you'd just go down the BOM and type:

=<hi1> x <w1>

=<hi2> x <w2>

=<hi3> x <w3>

But no, not really. Your problem here is using multibody, it's not particularly great for passing information onto the parts because they are essentially derived. 

Your better option is to use parts and assemble them in an assembly. Then you can set up a template with the hi w L in and the parameters don't need to be unique because they're contained in each part. 

If you are wanting to drive all your dimensions from the top assembly, the best way is to use a simple iLogic code, but this will complicate your dimensions idea which was the point of this post. 

As for your other question, just add a new one called 'dimension' This will create a custom iproperty. 

[drawingsCHR7R]

Understood, thanks for the help.

[rhasell]

Hi

You need to be very methodical, with your parts.

I use iLogic to create and populate the parameters in each part. My code will create the parameters of "length, width, height, thick and od" then populate accordingly.

I also have an additional two parameters of DIMa and DIMb for manual sketches, and these take priority when calculating perimeters and populating the fields.

See example based on your sample for reference.

[drawingsCHR7R]

Mmm, seems as though I definitely need to spend some time on this and upskill myself.

Thanks for the contribution.