Inventor Tube & Pipe Wish List Part 2

Originally Published 4/4/2014

Hello again all you happy people.

Sorry, I just like Droopy.

Anyway,  welcome to Part 2 of my Autodesk ® Inventor Tube & Pipe wish list.  I revamped the first post in this series to include links to the Autodesk ® Discussion Forum Idea Station posts for these suggestions, so I will do the same here.  Ready to go?

Tube & Pipe Branching

This request has actually been moved to the “Under Review” state in the Idea Station, which means that Autodesk is looking at whether this CAN be done, and SHOULD be done.  Progress!  Basically this is what I am asking for.  Currently, in Tube & Pipe, you create a branch by adding a branch fitting into an existing route, and then beginning a new route from the outlet of that fitting.  This works just fine, until you need that branch to line up perfectly with another pipe run, or a piece of equipment whose location is fixed.  See the image below; I need a line coming from the outlet of the pump and intersecting the main trunk line shown.  If I place a tee in this line, I would need to have an external reference point in my route to constrain the tee’s location to in order to ensure it lines up with the pump suction.  If the pump moves later, there is no guarantee that this reference point would move with it, and would result in a failed route.

Branch Location

My proposed solution is one I have seen in another piping program.  It would be nice if we could run a line from the suction nozzle of the pump and have it intersect the main line shown, and have Tube & Pipe place the tee automatically.  Perhaps this would mean that in our Tube & Pipe styles we would need to specify a branch fitting as well as the elbows we need to specify now.  I would be OK with that!  This could even work in the context of a single route, creating branches on the fly as needed.  If done in conjunction with one of my other proposals; the ability to have a route reduce in size; the branch fitting could even be a reducing tee, for example.  Here is a link to the Idea Station post if you want to add your Kudos.

Tube & Pipe Branching

Content Center Parameters Propagated to Tube & Pipe

A little over a year ago I posted an idea to the Idea Station about a problem I was experiencing with getting column information out of the Content Center Family Table and onto my part models in Tube & Pipe.  Here is a screen shot of the post:

Idea Station Post

I was going to include this in this wish list, but in the last few days I have had some great success on a work around for this problem.  Instead I think I’ll end this whole thing on a positive note and share what I’ve figured out in case it will help you.

To sum up what I was after, I wanted to get the same information onto the pipe spool model regardless of whether it was placed as part of a pipe run, or simply placed as a stand alone part.  The out of the box behavior was different in Tube & Pipe than when placing it loose in an assembly.  I wanted a concatenation of the spool type, nominal size and length.  The work around starts at the part level. I placed a pipe spool from the Content Center, “as custom”, and saved it as a stand alone part.  I opened up that part file and looked at the model parameters.

Pipe Spool Part parameters

In the parameters I scrolled down to “length”.  This parameter was first created as a part of the original iPart which was authored and published to be our flanged pipe conduit.  For help on creating and authoring your own custom pipes, see this Help document:

Author a pipe iPart

I set the length parameter to be exportable, then right clicked on the length value and selected “Custom Property Format”.

Custom Property Format

For my needs I wanted the value to show up in my iProperties and in my Bill of Materials as fractional inches.  I unchecked the Units String so that the “in” would not show up as a part of my file names later.

Custom Property Format Dialog Box

With these changes tucked away, I saved and closed the part, making note of where I saved it for the next step.  In Inventor still, I went to the Manage tab and opened the Content Center Editor.  Finding the family for this pipe spool in Tube & Pipe\Conduit\Pipes, I right clicked and selected “Replace Family Template”.  When the file dialog box opened I navigated to the location of the spool I had just modified and selected it.  After a few moments (with my fingers crossed) I got the satisfying “Published Successfully” message.  These changes to the parameters had now been propagated to the Content Center Family.

Next, I edited the Family Table for this pipe part.  Now, normally I use one column in a part family table to populate both the file name and the BOM description.  I do this by mapping the file name column to “Project.Description” under Column Properties.  For these pipe parts, however, this didn’t work.  The fact that I was getting different results in Tube & Pipe, versus placing the pipe as a stand alone part made it necessary to use two different columns to populate file name and description.  File name is a standard CC Family table column, so for this one I chose an Expression as shown in this shot:

File Name Column Properties.

To edit this, you right click on the column header and choose Column Properties.  The Expression string is hard to see but here is the text:  {DESIGNATION}&” ETFE SPOOL x” &{length}

Designation is set to our sizes for this pipe, expressed as 3 or 4 digit size codes (1″ – “100”).  The Length column has been set up as an Expression column as well as shown here:

Length Column Properties.

This allows Tube & pipe to place these pipe spools at any length in this range.  Note it is mapped to the iProperty Custom.Length, which will push the value of Length out to the part as a custom iProperty.

For the Description, I chose a column we were not really using for anything else, but you could just as easily create a new column for this.  In my case I used Stock Number.  I set up the Column Properties as shown here:

Stock Number Column Properties

Note how this is mapped to Project.Description to populate the part iProperty.  Again the text of the expression is:  =&{DESIGNATION}&” ETFE SPOOL x <length>”  This is slightly different than the File Name.  The “carrots” around length here will cause the resulting string to populate the part iProperties as an expression there, using the value of the custom iProperty “Length” as a part of the Description.  This will ensure that if the pipe route changes later on and the length is different, the part iProperty for the description will update automatically to the new length.  This was something I was trying to do for quite some time and finally hit on it.

So with this somewhat lengthy process, I was able to force my pipe spools to come into Inventor with the correct file name and iProperty information, regardless of how they were created.  A shot of the iProperty dialog for my test pipe looks something like this:

Pipe Spool iProperties

Note the file name along the top has the size, the type of pipe spool and the length.  In the Description field, I have set it to show you what the expression looks like, the value for it is the same as the file name.  Now, it is important to note that when routing pipes using Inventor Tube & Pipe, your pipe spool file names will be auto generated.  You can set your Tube & Pipe setting such that you will be prompted for conduit file names.  To do this, right click on the “Tube & Pipe Runs” main assembly in your Inventor browser window, and select “Tube & Pipe Settings”, then check the appropriate box.  I do this so that I can add the job number to each spool as a prefix.  It’s a lot of work up front, but I’m always glad I did it later when I need to use Copy Design.  Also note, that you can modify the file name that is generated by placing a pipe spool outside of Tube & Pipe, if you place it “As Custom”.

Well, this went from a wish list to a tutorial, and I’m sorry if I got long winded… but I hope there is something in here you all can use.  As for me I think it might be time to call it a week.


“Autodesk® screen shots reprinted with the permission of Autodesk, Inc.  Autodesk ® , AutoCAD ® , DWG, the DWG logo, Vault ®, Autocad Electrical ® and Inventor ® are registered trademarks or trademarks of Autodesk, Inc., and/or its subsidiaries and/or affiliates in the USA and other countries.”  Programs and programmers’ information used with permission.  Thanks guys!


CAD Department Supervisor at Powell Fabrication & Manufacturing, Inc. CAD Designer & Detailer specializing in Inventor Tube & Pipe, Frame Generator, Content Center, Vault Professional. Autodesk Expert Elite member. Blogger. Autodesk University Speaker 2014-2018. Husband and father. Photographer.

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