Better option for not using Tube and Pipe routing.

[cad]

Hello guys,

Have been working on AutoCAD for many years.

As I started working on Inventor this month and quickly getting familiar to it.

(Already finished most of advanced tutorials and quiet confident now).

BACKGROUND:

My company bought a Building Design Suit recently. So that doesn't include Professional version of Inventor.

As I searched, Tube and Pipe routing is not available.

So, I wanna know the perfect substitute for T&P Option.

Image attached here which is a sample design I make for Pumprooms.

WHAT I DID:

I already made all the fittings, Valves etc (which my company using) and added to content center.

Also Pipes added to Frame generator contents.

WORKFLOW:

1. Made PUMPROOM.ipt which includes only PUMPROOM Walls and floor.

2. Made MAIN_ASSEMBLY.iam

3. Placed PUMPROOM.ipt to MAIN_ASSEMBLY.iam

4. Also Placed All fittings (flanges, bends, valves etc).

5. Made few new WorkPlanes to locate the distances required for pipework AND constraint the fittings to New WorkPlanes.

6. Made a skeleton using lines connecting fittings.

7. Made a FRAME by using Pipes from Frame Generator contents.

LIKES:

It's now easier for me to change the distances by using WorkPlanes parameters.

Also easier to change the PIPE size and FITTINGS size.

PROBLEM:

It takes a while to make whole assembly by constraining every flange, gasket, bend, valve etc. (It takes less than half of the time for me to make 3D in AutoCAD).

It is more difficult while I am getting big modification. Like, whole route changed. (Suction line going throught front wall. And Discharge line comes out between two pumps with using TEE.) It forces me to re-constraint most of the flanges & fittings. And making Frame skeleton and FRAME again...

So, nearly making whole Assembly again. 😞

(However I can modify 3D-Pipework faster in AutoCAD)

Wondering, if I am not using the right workflow.

Please help me to choose the proper way that makes easier MODIFICATION later on. So I can move to Inventor from AutoCAD earliest.

Many Thanks.

[Mark_Wigan]

hi CAD,

 you are off to a good start but personally i would tend not to use the tube and pipe tools anyway for something like this. (i use that mostly for running flexible hoses, for moving parts where they are very useful).

i would keep your skeleton. it will be useful, but i personally wouldn't use frame generator to populate the runs. i will explain one method below. Sorry if it sounds long winded. i am sure it would be easier if i recorded this for you but i am away from my inventor atm.

1. copy your old skeleton / sketch ipt file. don't put any fittings in it though. you should setup nice easy to manouver workplanes in it, and run a series of sketches around on them as you need to represent your pipe system.
2. add a couple of parameters to this same ipt file. how many will depend on how much you want to drive the overall assy and parts from this skeleton file... eg "pipe1_od", "pipe1_wall_thickness" etc
3. be sure to tick the 'export' checkbox for each new parameter before you save the file. that way the parameter values will be available from within any ipt or assy that you link / derive your skeleton part into later on.
4. make a new assy, place the part in it & ensure that it is grounded. also, while you are at it, set the occurence of this newly placed part to be a "reference part" from your bom options, so that it does not get called up in your parts list later on.
5. you will be able to constrain fittings to parts of the sketch, or, to the features of pipe runs that you are about to generate, or other fittings that are placed.
6. lets make a new pipe run now from the skeleton. there are some tools in inventor to automate this next bit, but i will explain the actual steps... (the automated tools i refer to kinda run these individual steps in the background, and, you can learn those later on once you become familiar with whatever method you end up using in future)... so for now, just create a new ipt file, save it, derive your skeleton into it, go into your parameters window, tick the parameters you wish to link through from the skeleton, then...
7. place the new ipt file into your assy. Set its occurence at 0,0,0, (or use the inventor assy bonus tools to place it & zero it on the skeleton for you automatically).
8. make your skeleton invisible now, or disable it via the rmb context menu. That will help to make sure you will be working on the new part and not accidentally working on the skeleton when you are making your pipe geometry...
9. from within the assy, edit the new part, and either:
   
   a) make a straight run= just make a new sketch on the start of the run (pipe diameter outer wall and inner wall) & sweep it along a straight part of the skeleton. save the part. repeat this for every other straight run you want to model up (from item 6 above). note you can (save as) make a copy of the individual part you just made and delete the existing run, to make a new run if you prefer. either way, you are just making parts on a derived part sketch and placing them into the assy. (you can call any dimension that you linked to the skeleton earlier on).
   
   b) full runs= you can choose whether to make a long pipe run, from pipe inlet to pipe outlet point, running around bends, changing direction etc for the run. you can even choose to make several sweeps within the same part that represent changes in pipe size, create lofts and other things. it depends whether you intend to use fittings or features in your top level assy. it is up to you.

after doing those runs, you will have placed them into your assy. you will have placed fittings, pumps etc reducers bends if you wanted to. you can change the skeleton and any parameter values you originally established. after which, you can run an update from your assy and see everything change for you. hit save to keep the changes.

hope this helps. there are many ways to do this. like autocad, it means trying a few ways and seeing how others do things so that you can develop your own good ideas.

[cad]

Thanks Mark,

That's a great help for now... 

So now I got some more ideas I never thought.

I understand that I need to try different options at an initial stage. And I will get the right way.

So, better to start as per your suggested way. 🙂

Many Thanks again. !!! 

[Mark_Wigan]

you are welcome any time.

Just drop us a line if you got any ideas or questions whenever you want.

[josh]

I have been doing pipe runs around a mine site with bog standard solidworks for the last 3 years and we were using a similar method to the one mark has mentioned. due to the indecisive management we needed to com up with a plan that would mean we could make big changes as fast as possible. some times completely redo the job from scratch in short notice.

what mark has described is called top down modelling and imho would be your best approach. i haven't tested the method we were using in solidworks with inventor as it requires 3D sketches as its main function and that isn't great in inventor. but there are other methods that might work just as well all be it a little more long winded than using a 3D sketch. i can think of any reason it wouldn't work in inventor.

due to the fact i haven't tested the method in inventor i won't detail it out here, but i will go through the thought process we went through when setting up the systems and parts for use etc. and some of the major benefits you can get from using inventor over AutoCAD.

the first question you should ask yourself is what are the drawings you want to produce and what information you want in them. the biggest advantage inventor has over cad is you can store a part and assembly files that have a HEAP of information included in it. so for example, you can have sizes, materials, visual styles and notes, to name a few things, stored in the part or assembly file that you can extract at a few clicks in a drawing instead of typing the same note over and over when you do a new drawing of the same part or assembly. you can also have multiple instances of the same part at different sizes in the one part file and things like notes update accordingly when the size changes. so for instance if a pipe goes from DN50 SCHD 40 to SCHD 80 DN65 your note will update with the right information automatically and you don't have to go through and correct each drawing. that is where the real time saving comes in imo.

the smart thing to do is take the time at the start and build a library of parts and assemblies that have all the information in them that you want. (which it sounds like you have anyway). do your most common stuff and then build on that library when you need to do a job with the not as common stuff. and don't fall into the "we just have to get this job out" trap. it takes 20 minutes longer to do it right, it is done then and never has to be redone so will save you far more than 20 minutes down the track. these parts can then be used in every assembly you use meaning you don't have to redo work. again a big time saving over CAD quite often. the biggest key to building a good library is think about what you want to see in the drawing while doing the part.

once you have worked out what the drawing is you want to produce and you have your library of parts and assemblies ready to go doing individual jobs is actually quite quick. in the case of the mine site i was on we cut drafting and modelling time by as much as 75% for most jobs. and they were already working in solidworks. they just didn't have it set up. basically we went from using sweeps and individual pipe components to using "prefabed" assemblies and then driving the assemblies off the driving sketch. it works amazing well and is super fast once you have the work flow down. i have used cad for a long time and if you put equal effort into setting up CAD and inventor you will get things done faster and better in inventor then you ever will cad. you can do it faster in cad because it is what you are used to and know. you have a huge learning curve ahead of you with inventor but the pay off is worth it 1000 times over if you set it up right.