Volume of Media in Pipes

Been playing with this for a while, but never had time to fully test it and get good results but it’s been itching me cause I knew the is a better answer to the existing solutions on the net.

                The question is: How do you calculate the volume of media in the pipes, or in any equipment for that matter.

                Every single video, blog or forum post I’ve seen are dealing with single pipe with open ends and while that’s good info I find it purely theoretical because you are never going to measure the volume pipe by pipe. Most of these solutions rely on copying the inside surface of the pipe, trim and stitch them back together along with capping the ends, and them sculpt-convert them into a solid that has a volume and for which you can assign material.

                My mind went straight away to derive, combine, sculpt, or possible extrude with intersect to better, faster do this on complete Tube and Pipe assemblies, not just individual pipes. I can’t expect any of you to manually do this because I know I wouldn’t.

                By far, over 10 clicks and multiple minutes wasted for the next best thing, by far, the fastest method I found to be a double derive with simplification and combine. We derive the assembly into a single body, then we use Revit BIM simplify to fill the voids (this is the fastest way) , we derive the assembly again as a different body and then we combine the both removing the second out of the first one which in fact will give us just the media inside the pipes.

                So for the first step prepare your assembly, remove components you don’t need or that will not influence the result to speed up the process and once done save that as a level of detail or design view. If you don’t want to edit your original T&P assembly then do a save copy as and work on that one.

                Open a new part and save it, then use derive component and select your assembly but in the select dialog use the options button and select your level of detail. You can do this later by changing it in the derive window as well.

  TIP: Save your new ipt before derive. I found it to be the problem with long compute time and crashes.

                In the derive style type choose “single solid body” and take off some of the stuff that will not help, like gaskets, bolts, nuts, pipe clips, etc. You should have done this on the assembly when you setup your level of detail or design view but you can do it now as well. Do not mark anything in the Options tab.

                The simplest, fastest way to fill the inside is to use the Revit BIM simplification tool that has a fill voids command we will use. You need to make sure it’s loaded in your add-ins and that you have a tab called BIM in your assembly or part environment. Use fill voids but don’t choose Auto Select because it will try and fill every possible pocket, hole and gap and it’s not relevant to us. Pick your open ends and click OK.

                Before selecting your edges or faces to fill you might want to do a bit of planning. If you select the top most edge / face you might end up with too much info like I did. Instead of selecting the outside of the tee I need to select the base of the up segment otherwise I will get the pockets in the reducing bushing which I don’t need.

                The good about my solution is that you can have as many routes as you want and they don’t need to be connected for this to work.

                Now you should have one single body with all pipes filled in so the next step is to bring in the original one back again. Repeat the steps above to bring it in as a new body.

                Use “combine” and specify the first body as your Base and the second body as your Toolbody, mark cut as your type of operation and click ok.

THAT’S IT!

                Depending on the edges, faces, you selected in the simplify operation you will have different results but now you can assign a material and verify the volume. Right click on the body in the browser or got to iProperties.

                Make sure you specify a material for the body otherwise it will show different Mass; volume will be same but you will scratch your head trying to figure it out why Mass is different on the body than on iproperties.

               

                Limitations:

                If you are using the default Content Center elbows you will need to re-author them. I have done it long ago because converting all my assemblies to neutral formats for clients or sending it to Showcase would unrecognisable twist them and this method of volume measuring will not work. Not all families are created like this and if you have errors simplifying the model then I would investigate the elbows you are using.

                Some elbows have the middle section done as a revolved but because Inventor fails to do a revolve, the axis has been offset by 0.01mm which in fact leaves your elbow with disconnected sections. If you zoom in on your elbow you will see that there is a gap in between the middle section and one of the ends you need to fixe and replace the family member. Or at least the very instance used in the assembly

                The proper way to do the middle section is by using sweep which doesn’t produce a gap in between consecutive segments. If you want to simplify it even more do a single sweep on the outside and another one on the inside, 2 sketches 2 features instead of 3 as it currently has.

Next post will be on how to calculate volume in various shape and size tanks.

Managed to add the video.... enjoy

Later,
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