Originally Published 5/14/2014
Hello all. As usual it’s been a while between posts. This has been the busiest year that I can recall at this company I work for. This is a good thing, but it takes me away from writing, and I do enjoy this. Still, I’d hate to have more time to write if it meant I didn’t have a job anymore.
Anyway… this post is going to be about Autodesk ® Inventor Tube & Pipe Styles. How to create them, where to save them and how to copy them. It seems pretty straight forward, but I’ve seen a lot of questions in the Autodesk ® Community Forums about how to do this, and I remember from when I first started using Tube & Pipe, that it was not immediately obvious how to go about setting these up.
First thing, let’s talk about “piping runs.iam”. This is an Inventor, “out of the box” file that is generally found in your install path, in the Design Data folder. This file may be placed in a shared drive, as a part of moving the entire Design Data to a shared location. Bear in mind that if you do so, you need to modify the Design Data search path in your Inventor Application Options.
This is the file that contains everything that Inventor Tube & Pipe needs to know to create pipe runs and routes. So, this is your Tube & Pipe environment “template” file… if you will. Here is the best place to add new Tube & Pipe styles, if you want to be able to use them all of the time. So many times, I see the question “Why aren’t my styles there when I start a new pipe assembly”. Most likely it is because the styles were created within a design, and not saved to this “template” file. I should point out that in this folder there are sub-folders containing English unit and Metric unit versions of the file… if you should want to use those.
Once you have opened this assembly file, select the Tube & Pipe tab on the ribbon, and then Tube & Pipe Styles.
|Tube & Pipe Ribbon|
The “out of the box” Tube & Pipe styles window will look something like this (Inventor 2013).
|Tube & Pipe Styles Window|
The toolbar along the top will help you create and edit your own custom styles. Here is a blowup of the tools:
To create a custom style, simply use New, or Copy an existing one that looks close to what you want. If you would like to create a new category, that’s very simple as well. Create a New style, and give it a unique category name. Once the style is saved, the new category will be created. Once you have selected New or Copy, the new style will be created under whatever category your currently active style is in. The active style is distinguished by it’s name being in bold text. If you use the Copy command, the new style will appear directly below the style you copied from, and will include _Copy (1) at the end of the name. You can simply edit that out and name the style whatever you want.
|New Tube & Pipe Style for Editing|
Your newly created style opens in a dialog box similar to the one above, waiting for you to fill in the information. Give the Style a name and a Category name, or accept the current category name. Categories may be created for things such as different materials, pressures, fluid codes… however you want to differentiate your pipe styles. Each style within a category may be named however you would like; suggestions would be to include the size, material or spec, and perhaps end treatment. But this is up to you or your company standards.
Once you have a style and category name, you need to specify the base fittings for this style. Decide whether this is going to be a Flanged or Butt Weld style. I will not be talking about Self Draining or Mixed Unit styles, since (frankly) I know very little about them. If your style is going to include or allow any flanged valves, fittings or instruments check the Flanged box. This will make it so that the gaskets and mating flanges are inserted automatically anytime you place a fitting or instrument that has flanges on it. Butt Weld allows for another setting which I will get to in a while.
You must specify fittings to be automatically placed in this style, based on which boxes you have checked above. If you have checked nothing, you will need to specify: Pipe, Coupling, Elbow 90 and Elbow 45. For Flanged: Pipe, Elbow 90, Elbow 45, Flange and Gasket. If only Butt Weld is checked: Pipe, Elbow 90 and Elbow 45. This assumes that you have these fittings defined and in your Content Center already. To create, Author and Publish these please see Autodesk ® Inventor’s Help documentation. Perhaps I’ll write up a walk through for these next.
When you double click inside one of the empty fields under the fittings, a Library Browser opens which has already narrowed your choices to the type of fitting you are adding. You can further narrow the results by adding filters and selecting the filter button at the bottom (looks like a funnel).
|Style With Fittings Selected|
Now that this section of the style is filled in, select the Rules tab to complete the final steps. You must specify a Minimum, Maximum and Increment length for your pipe spools. These can be whatever fits your specs, but I do have some advice. For Minimum I almost always go with .001″. This allows me to create extremely small gaps between fittings if I need to. With the piping I run, I sometimes need to have 2 small branch fittings in the same spot 180 degrees apart. This setting allows me to have 2 route nodes that are .001″ apart, which rounds out to nothing on a fabrication drawing. You will know what is going to work best for your situation. Maximum is usually dictated by the longest length of tube or pipe that you can buy. In my case this is 240″ or 20′. Increment specifies the increment by which your pipe lengths can grow. For example, you can specify that you always want your pipe lengths to be within the nearest 1/2″. For me, I again set this to .001 so my pipes can be whatever length they want based on equipment layouts.
If you selected Butt Weld on the General tab, your rules page will look like this:
|Rules For Butt Weld|
Here you can specify a gap between welded pipe and fittings, based on your welding specs. This will ensure proper cut lengths in your BOM. You can also choose whether or not to display the gap in your models. In any style where flanged is set as an option, but is not the only option, you will see the Coupling Type pick box. This gives you the option to have the system place a set of flanges and a gasket at any point that would require a coupling, such as on pipe lengths which exceed your maximum setting.
When you have set everything in your style to what you want or need, hit Save and your new style will be created. If you have given it a new Category name, the new category will also be created. Now that you have one style done for this new category, you can copy it as many times as needed for the various sizes, and simply change the size setting and name as needed. In this way you can quickly create an entire family of tube & pipe styles.
The Export & Import buttons on the tool bar can be used for just what it implies. Tube and pipe styles, or categories can be exported to a .xml file. If you feel comfortable with doing so these can be edited outside of Inventor and then imported back in with the changes. I have used this to quickly copy a category, saves it for a different fluid code and change the color in the .xml file (using find & replace). I don’t recommend this for the faint hearted or those not at least somewhat familiar with .xml files. This Export/Import feature also allows you to copy styles between machines that do not share a common server. Simply export them and put some portable media, and Import on the machine that needs them.
So, there it is. A quick (sort of) walk through to get you started in creating Tube & Pipe styles for Autodesk ® Inventor.
“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!