Ask The Experts: Isometric Pipe Spool Drawings

[jeanchile]

Hello All,

I have been asked by one of my clients to provide an isometric piping diagram for a product that we have modeled/developed for them. We have already provided models, review drawings, design drawings, and fabrication drawings for this product but what they are looking for is a simple isometric pipe diagram where they can hand write their weld test data and put the material data sheet number references. I have submitted a sample of a drawing we completed with an isometric view of this piping as a full view (iso view created by IV) but they are requesting something simpler like they are used to (one-line iso pipe spool-type thing with symbols instead of modeled valves, etc.). I am embarking on a process to get them to change their standard but I was wondering what you experts thought while I am doing this (in case they refuse).

I don't want to create drawing that isn't tied to the model somehow for obvious future-revisions-parametric reasons so I was wondering what you think my options would be for keeping this all in IV (instead of just doing something seperate in AutoCAD.

Any suggestions / ideas? Thank you in advance for your help with this.

[DonovanCox]

What they want is similar to what a program called Isogen does, Inventor has the capability to output in a format that isogen reads, but i've not had good results doing so. Edited by: donovan.cox@ecadinc.com on May 25, 2010 10:24 AM

[jeanchile]

Looked into Isogen program, thank you. Unfortunately, not something I am going to go for. I can't justify the expense for this one project plus it defeats my purpose of having the drawings linked to the model. This design will see a few different iterations and revisions and I was trying to avoid having to use a different program. If I am going to do that, I'll just use AutoCAD or make a new "one-line" model in IV.

Does anyone know if it is possible to have a 3D sketch show up on a drawing? I've never tried. Maybe I could do something like that. Anybody else have any other ideas?

Thanks again for the input!

[trevorauman]

We have had the same issue. We tried tying centerlines to the pipe sections, but the dims didn't know how to parse the isometric view. So we tried applying axis to each of the pipe in the 3D Inventor model and dimension off of the axis (you can make the axis appear by expanding the .iam for the view and selected "include" from the right-click on the items that don't show in the drawing view, works great for elevation in the model you want to show in the views on the drawing driven fromt he model!) Neither worked. We are currently trying to work around it another way using a 3D sketch that is the structure of the .iam for the pipe spool so that they are tied together but the Inventor .idw again can't parse the isometric views dimensiosn of lines, only physical surfaces. I'll let you know if we find anything.

[graemev]

"Does anyone know if it is possible to have a 3D sketch show up on a drawing? I've never tried. Maybe I could do something like that. Anybody else have any other ideas?"

Yikes!

The best I can think of is to make very narrow rectangles, "flat donut" sectors, etc. and extrude them as wafer thin plates.  Orient each piece with the ultimate orientation of the ISO view in mind.  You should then be able to dimension to the model edges on the drawing.  There is potential for making these dummy parts associative to the original assembly.

It's an ugly solution, I'll admit.

[trevorauman]

Alright, I have a possible solution, not sure how well it will work with what you have. When you create an .ipt with only sketches there is an option when you right-click on the sketch in the Browser Bar to "Export Object". If this is turned on the sketch will show in the .idw. Unfortunately it does not appear to function if there is a Solid Body in the .ipt. If you include one of these Sketch Only .ipt into an assembly it automatically comes in with the visibility turned off. If you turn on the visibility the sketch is shown as a child of the .ipt, right-click on to he sketch and select "Include" it shows up. I have not tested the it too far, but it appears that the dims that are attached are correct on the sample piece I used.

Tada!

If I were doing a pipe spool I would create a 3D sketch for the "skeleton" and then use the user created and origin axis and planes to tie the pipe fitting .ipt's to the 3D sketch .ipt so that they move together.

The idea of tube and pipe is cool, but it is my opinion is that they went about it all wrong. It should be a 3D Sketched based system, with line properties as the pipe size and special nodes inserted representing valves and what not. Then the 3D sketch would be used as the ISO and the cool programming they set up to automatically create the pipes would reference the sketch. As soon as a line was broken it would require info for the break, valve, reducer, etc and if a 90 degree or T were present it automatically put a fitting here. Well maybe 20 years from now we will look back and laugh at the frustrations we had trying to integrate Inventor with Plant 3D and AutoCAD...