Attn: Tube & Pipe Genius' - cbenner are you out there?

[jeanchile]

Hello Chris (or anyone else who has input really),

I've been recently tasked with investigating the use of Tube and Pipe for our skid designs and have come across many of your informative posts on the matter. Let me first thank you for being such a valuable asset to this community. You're answers are always complete and very helpful and, for someone digging around on the site, it makes using older posts like that very easy.

I am wondering if you have any more advice for someone looking to implement this tool into their workflow. The gems of wisdom I have come across (and copied into my research notebook) so far are:

1.) Always constrain your routes to the main assembly planes

2.) Avoid AutoRoutes at all costs (I'm not sure why yet)

3.) Fully constrain your 3D sketches but find a way to allow necessary degrees of freedom (revisions)

4.) Be prepared to rebuild routes on occasion

5.) Use the "Piping runs.iam" template to create every conceivable rule then you can delete the ones you don't need out of your current file

6.) Devise a system for placing CC components into a route that makes sure you get the right one

7.) Rough in the route with a 3D sketch and then lock it down with dim's and constraints

I am going to apologize for my ignorance in advance as this is a tool that I have just started seriously investigating. Questions that I have:

1.) Do you draw independent 3D sketches for your routes somehow or are you using the "route" command for your 3D sketches (I think you have to use the "route" command but I don't really know)?

2.) We hardly ever use 3D sketches so I'm curious how you use geometric constraints on your 3D sketches? When we have used 3D sketches in the past we always follow JD's suggestion of using a 2D sketch to control them. I'm not sure that works in the T&P environment.

3.) I've been through the T&P tutorials and I've read the chapter in Curtis' book but I'm still not sure how you are able to draw the route first with no dimensions, can you elaborate on that? It seemed from the tutorials that I was right-clicking and entering numbers a lot.

4.) What advice do you have on allowing the predictable degrees of freedom in a design? I'm not sure I completely understand how you do this (especially if I am entering dimensions as I go).

5.) I remember seeing somewhere that you named your styles off of an "in-house" specification and then end treatment and then size. Is the size you use the NPS or is it an ANSI pressure class or schedule?

Thanks (to you and anyone else who would like to chime in) for all of the good information!

[salariua]

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@jeanchile wrote:

1.) Always constrain your routes to the main assembly planes

- That's right. if you drag them by mistake in the main assembly you will loose a lot of hair before figuring it out.

2.) Avoid AutoRoutes at all costs (I'm not sure why yet)

- They tend to automatically reroute themselves without a warning so even if you connect two fittings with autoroute right click on it and convert to sketch.

3.) Fully constrain your 3D sketches but find a way to allow necessary degrees of freedom (revisions)

- Same thing with constraining routes. They get skewed or move around. 

4.) Be prepared to rebuild routes on occasion

5.) Use the "Piping runs.iam" template to create every conceivable rule then you can delete the ones you don't need out of your current file

- I don't have any style in my "PIping runs.iam". I did export each style in it's own xml and import them when needed. I have an xml for PP, ABS, PVDF, PVDF-HP, Stainless, etc. So I only import the style needed.

6.) Devise a system for placing CC components into a route that makes sure you get the right one

7.) Rough in the route with a 3D sketch and then lock it down with dim's and constraints

- As soon as you click on route and have created the first line , right click and disable Auto-Dimension. I always dimension mines after drawing the sketch. Say you have point snap on and you have the mouse pointing on a wall (or any other reference) and you type -100 (to have it 100mm from the wall), it dimensions the length of the route instead of dimensioning 100mm from you reference.

I am going to apologize for my ignorance in advance as this is a tool that I have just started seriously investigating. Questions that I have:

1.) Do you draw independent 3D sketches for your routes somehow or are you using the "route" command for your 3D sketches (I think you have to use the "route" command but I don't really know)?

- I always use the route command, I like the “3D Orthogonal Route Tool”. I even use it to draw my 3d sketches for frame generator.

2.) We hardly ever use 3D sketches so I'm curious how you use geometric constraints on your 3D sketches? When we have used 3D sketches in the past we always follow JD's suggestion of using a 2D sketch to control them. I'm not sure that works in the T&P environment.

- Orthogonal Route Tool and use the constrains available like: collinear to align lines on same level, perpendicular and parallel to constrain lines to projected geometry (plane origin) etc.

3.) I've been through the T&P tutorials and I've read the chapter in Curtis' book but I'm still not sure how you are able to draw the route first with no dimensions, can you elaborate on that? It seemed from the tutorials that I was right-clicking and entering numbers a lot.

- You click on a circular edge or point to start your route and when the 3D Ortho Tool appears you move your mouse on one of the axis (of the ortho tool) and type a dimension to go in that direction by that value.

4.) What advice do you have on allowing the predictable degrees of freedom in a design? I'm not sure I completely understand how you do this (especially if I am entering dimensions as I go).

5.) I remember seeing somewhere that you named your styles off of an "in-house" specification and then end treatment and then size. Is the size you use the NPS or is it an ANSI pressure class or schedule?

Thanks (to you and anyone else who would like to chime in) for all of the good information!

Forgot to men that if you need to demote a sketch turn the visibility on and start deleting constrains. You can also insert 2 node points on a line and delete the one in between to split the original ones.

[cbenner]

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@jeanchile wrote:

Hello Chris (or anyone else who has input really),

I've been recently tasked with investigating the use of Tube and Pipe for our skid designs and have come across many of your informative posts on the matter. Let me first thank you for being such a valuable asset to this community. You're answers are always complete and very helpful and, for someone digging around on the site, it makes using older posts like that very easy.

I am wondering if you have any more advice for someone looking to implement this tool into their workflow. The gems of wisdom I have come across (and copied into my research notebook) so far are:

1.) Always constrain your routes to the main assembly planes

2.) Avoid AutoRoutes at all costs (I'm not sure why yet)

3.) Fully constrain your 3D sketches but find a way to allow necessary degrees of freedom (revisions)

4.) Be prepared to rebuild routes on occasion

5.) Use the "Piping runs.iam" template to create every conceivable rule then you can delete the ones you don't need out of your current file

6.) Devise a system for placing CC components into a route that makes sure you get the right one

7.) Rough in the route with a 3D sketch and then lock it down with dim's and constraints

I am going to apologize for my ignorance in advance as this is a tool that I have just started seriously investigating. Questions that I have:

1.) Do you draw independent 3D sketches for your routes somehow or are you using the "route" command for your 3D sketches (I think you have to use the "route" command but I don't really know)?

I always use the routing tool in Tube & Pipe.  As mentioned in the other reply, the orthagonal routing tool will help direct you.  but avoid auto routes, always convert them to sketches and use dimensions and constraints that YOU choose, to control your routes.

2.) We hardly ever use 3D sketches so I'm curious how you use geometric constraints on your 3D sketches? When we have used 3D sketches in the past we always follow JD's suggestion of using a 2D sketch to control them. I'm not sure that works in the T&P environment.

When using the routing tool, you can "Include Geometry" to bring in work features suck as edges or planes, from your surrounding environment (ie frames [I know you are familiar with those!] or other pieces of equipment).  Once you have included these work features, use them to place dimensions and/or constraints that will control your route sketches.  Be advised, these become independant of the original work feature.  So if you chose a frame surface to include a work plae, and the frame changes... the work plane stays where the original surface was that you included.  As long as you know that, you should be ok.

3.) I've been through the T&P tutorials and I've read the chapter in Curtis' book but I'm still not sure how you are able to draw the route first with no dimensions, can you elaborate on that? It seemed from the tutorials that I was right-clicking and entering numbers a lot.

Generally, when I start a route (and this is not nocessarily the right or only way), I place my end fittings such as flanges on a heat exchanger or pump, etc... then use these as the starting points of my routes.  I simply sketch a dummy path that is similar to the path I need to follow for that route.  I then delete all of the dimensions placed by Inventor, include whatever geometry I need, and start adding my own dimensions and constraints until the route is what I need it to be.  Short routes can be done by simply picking the two end points and letting Auto Route choose a solution for you... toggle through using the "select other" tool and choose the solution you like best.  Then IMMEDIATELY conver the Auto Route to a sketch,a nd add your own dimensions and constraint.  Never let Inventor control your sketches for you.

4.) What advice do you have on allowing the predictable degrees of freedom in a design? I'm not sure I completely understand how you do this (especially if I am entering dimensions as I go).

Following the routing advice above, use more constraints than dimensions... leaving as many "legs" of your route as possible un, or under dimensioned.  As long as they are constrianed geometrically, you can have a fully constrained route with a minimum of dimensions.  Doing this will allow your route to grow or shrink as needed when you move equipment around.

5.) I remember seeing somewhere that you named your styles off of an "in-house" specification and then end treatment and then size. Is the size you use the NPS or is it an ANSI pressure class or schedule?

An example of one of my style names is:  TIBW00 800 Bleach.  TI = Titanium  BW = Butt Weld  00 = Numerical Spec that refers to an internal document that details what fluids, temperatures, ratings (150#, 300#, Pipe Schedule etc) and fasteners are allowed on this spec.  800 = 8" pipe size (ANSI), and the Fluid is specified only because I like to give different fluids different colors... for my own use more than anything else.  For example when I see a red pipeline I know it's a bleach line... just makes it easier to track things in complicated assemblies.

Thanks (to you and anyone else who would like to chime in) for all of the good information!

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Hello,... sorry to get back so late... I've been swamped with actual piping design lately.  Thanks to salariua for chiming in and offering some great suggestions!  I've added my meager comments above.  (btw... genius?... hardly... lol!)

btw... my blog has a lot of suggestions as well, and recently moved to a new host.  I make nothing from it, I do it just for fun.  Feel free to check it out and leave comments.  See my signature line.   Hope I could help!

[salariua]

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@cbenner wrote:

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Thanks to salariua for chiming in and offering some great suggestions!  I've added my meager comments above.  (btw... genius?... hardly... lol!)

It seems we're following same "best practices". I am in no way trying to step in your shoes (genius), just fill in the gaps 🙂

[cbenner]

Adrian, my friend... keep jumpin' right in there!  I know just enough to be dangerous... someone has to show up and tell me when I've got it wrong!

[salariua]

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@cbenner wrote:

... I know just enough to be dangerous... 

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Dangerous and Wanted for your skills. 

[jeanchile]

Chris, Adrian... I can't thank you both enough for the information. This was exactly the kind of thing for which I was hoping. And, don't be modest, you are both considered experts on this forum because you have demonstrated it time and again. I'm sure I'm not the only user here who values the information you've laid out for us. That being said, I do have some follow up questions if you'll permit me:

@cbenner wrote:

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 Be advised, these become independant of the original work feature.  So if you chose a frame surface to include a work plae, and the frame changes... the work plane stays where the original surface was that you included.  As long as you know that, you should be ok.

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SERIOUSLY!! I hope I am misunderstanding your statement because what is the point of allowing their inclusion then anyway? It would appear from both of you guys' comments that the only "adaptive" parts of a route are the start and end point plus any dimensional/geometrical constraints I put on the sketch. If I have a hole through a part of my skid frame (done in frame generator) and I include that hole geometry in my route are you saying that it won't update if the hole moves? Because this kind of thing happens ALL the time in my office. I'm just trying to understand which parts of the routes will update and which won't. So if I am left with a choice of using an edge, workplane, or just dimensions, I know which ones to use. If I have to write procedures that forbid the inclusion of an edge or hole or something we'll find another way, but it seems to "fly in the face" of what makes Inventor usable.

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@cbenner wrote:

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...800 = 8" pipe size (ANSI)...

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So then if I guess at an extrapolation would 10" be 1000 and 2 1/2" be 250? I'm not saying I'm going to do it this way, just curious about it as I determine our process. We usually name our database items, lists, etc., using standard filtering methods (i.e. using the lowest number of parameter values first, then the next lowest, etc.). We usually end up with fewer mistakes that way. That means if I follow your example I would use the end-treatment first, fluid second, then the spec, then the Pipe Size but that seems backward. I'm going to have to spend some more time on this part.

We have a general piping specification that has the overall information about piping fabrication and design in general, then we have individual piping material specifications for different kinds of line types. Each material specification covers the Design Pressure, Design Temp, Product, and Piping Material, summed up as a "Service". If any of these change, it's a new specification. The issue I am trying to resolve is that we might have several different wall thicknesses (schedules) of pipe in the same specification (e.g. our spec 3CSBUXXX might have schedule 80 pipe below two inch, schedule 40 pipe from 2 to 12, and schedule 20 above that). If I've got my information correct, because I have a new style for each size, I could have hundreds of styles once these are all set up .

Nothing we do in this regard is different from what anybody else in the process piping industry does. Wouldn't it be nicer if T&P followed a similar process to that? It's my understanding that Plant 3D works that way. We would have 40 or so specifications to set up instead of 1,040 styles.

I am also shocked that T&P won't allow for branching off of a line. I'm still unsure how to create those kinds of routes so could one of you confirm that it has to go like this:

1.) Create the run route.

2.) Insert a fitting (e.g. reducing tee) where the branch occurs (I have no idea how to constrain this yet).

3.) Use the fitting as the starting point of the new branch route.

Our normal process would be to sketch out the centerlines of all the routes first but I can't do that until the branch fitting is in there right (good criminy I hope I am missing something here)?

Thanks again guys, go tell your bosses I said you get a raise.

[salariua]

The runs will adapt to your included geometry as long as you don't change it! if you change the frame members (replace) then the reference is not there anymore just like normal Inventor behavior.

The change size (in frame generator) should maintain references because the member faces should be the same. You drive a sketch and extrusion via table.

There are 3 ways of doing branches:

1- insert node (and control it's position with dimensions), then place tee with place fitting (on your mouse to drop wherever available, like our node or a pipe end). start another route from that tee.

2 - draw the branch as part of the original route but don't connect end points (inventor won't allow it).

3 - place and constraint the tee and have your runs from it.

[salariua]

I just had a thought about it. I haven't done any frame generator referenced routes but here's how I would do it.

I would do the frame skeleton as extruded surfaces (don't know if that's an option for you, maybe you do the skeleton form other references as well, instead of building sketches and extrusions) and I would use the skeleton faces as my references for the runs.

This way if you decide to change your frame member shape (ex: from square hollow section to circular hollow section) you would still have the references in place for your routes.

[cbenner]

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@jeanchile wrote:

SERIOUSLY!! I hope I am misunderstanding your statement because what is the point of allowing their inclusion then anyway? It would appear from both of you guys' comments that the only "adaptive" parts of a route are the start and end point plus any dimensional/geometrical constraints I put on the sketch. If I have a hole through a part of my skid frame (done in frame generator) and I include that hole geometry in my route are you saying that it won't update if the hole moves? Because this kind of thing happens ALL the time in my office. I'm just trying to understand which parts of the routes will update and which won't. So if I am left with a choice of using an edge, workplane, or just dimensions, I know which ones to use. If I have to write procedures that forbid the inclusion of an edge or hole or something we'll find another way, but it seems to "fly in the face" of what makes Inventor usable.

This has always been the case for me, but I'm going to look into what Adrian has posted below.  Genius that you say I am, maybe I've been doing it wrong all this time.  

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@cbenner wrote:

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...800 = 8" pipe size (ANSI)...

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So then if I guess at an extrapolation would 10" be 1000 and 2 1/2" be 250? I'm not saying I'm going to do it this way, just curious about it as I determine our process. We usually name our database items, lists, etc., using standard filtering methods (i.e. using the lowest number of parameter values first, then the next lowest, etc.). We usually end up with fewer mistakes that way. That means if I follow your example I would use the end-treatment first, fluid second, then the spec, then the Pipe Size but that seems backward. I'm going to have to spend some more time on this part.

You extrapolated correctly.  We took this format from somewhere, long before I came on board here... so i have no idea of the source.  Must have copied someone elses specs as a benchmark.  We are revamping our actual pipe specs right now so that they include the material, end treatment, schedule, rating, gasket and fastener spec.  For example a 316SS butt weld, schedule 40 150# with B7 studs might look like 316BW40A11.  Our engineers built a great self building table in Excel, where you pick each category from a pull down list and it builds the spec for you... love it.

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[lesmfunk]

And for beginners, be aware of the lying "Save" button. You'll figure out very quickly that your files are not actually saved until you exit out of the run and save the top level T&P assembly.

Also, when part numbering, you can get the length of pipe to drive into the part number by including "PL" or "L" in your part number expression in Content Center. Then, you have to right click your populated route and select change size and then click OK. (Do not actually change size)

[jeanchile]

Thank you Adrian for the clarifications and the suggestion on the Frame Generator surfaces. I'll add that to my list of things to test.

[jeanchile]

That's good information there lesmfunk and something I'll add to the procedures I may write here in the future. It seems a little similar to the Frame Generator tools in that they will generate all of the files and components but none of them exist as files until you exit to the top and save them all.

I have to be honest here though and voice my general disappointment in this tool. I was hoping for something that was a glaring improvement on the way we are doing it now. It just seems to be so "unfinished". And that is to say nothing of the lacking documentation and confusing nature of the tools. At this point in my study I'd say there's a solid 60% chance we won't even be able to use this functionality of the software but I'm hoping that improves over the course of this exploration.

I recently sat through a Solidworks demo on their routed systems and that may have something to do with my dejected demeanor. I realize that is was a demo, and we weren't anywhere near digging down into the "nitty gritty" of the tools, but it just seemed SO much easier over there. It's kind of a downer.

[salariua]

Hey you frame generator users, you might like this: http://forums.autodesk.com/t5/inventor-general-discussion/ipart-creation-problems/m-p/5374555#M52667...

It' probably nothing new but worth refreshing, the whole thread worths checking.

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jeanchile wrote:

I've been recently tasked with investigating the use of Tube and Pipe for our skid designs

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Glad you're doing it the right way, 1 minute in planning saves 5 in execution but don't antagonize to much. Start working, it's far better experience to learn and discover this yourself. Each to his own method and don't get disappointed about Inventor Tube and Pipe, before even started. Besides you are comparing our list of Beware and Pitfalls with a marketing demo.

I hope you just realised what you made me do.... I went over to the dark side (SW) to see some demos, I even watched some youtube videos in spanish. They will be spamming me with emails and adverts everywhere I go now.

Someone told me that the best software is: THE ONE YOU KNOW, so if you company uses Inventor, go with that, draw from other Inventor modules as much possible.

I would try and do it in both software, get an expert of each software to do one of your products.

Edit:
I just watched a long video on youtube for SW and it didn't impress me but maybe the functionality is there and it's hard to see. The presenter was having a hard time changing a fitting orientation (min 47) and i wonder how do you go about having a weird positioning angle like 37.5 in SW , he didn't seem to be able to drop a fitting (valve) anywhere on the pipe, but had to create a point first. I liked the idea of having the pipes as virtual pars inside the assembly, my biggest pain is waiting for the files to be saved but if you wanted to make a drawing of the route you had to change it from virtual to on disk, back to square 1.

Are you kidding me? Look at what ordeal David (sw certified expert) has to put up with to rotate a flange and he doesn't seem to be able to change it afterwards, it needs to be done exactly before doing a route.

I did liked the automatic size change when dropping a reducer in line, and the branches, Chris has been asking for this functionality for a long time.

I bet you will relize that tube and pipe for AIP and SW are quite the same in the end, in terms of effort you need to put in.

End Edit.

[cbenner]

For us, one of the big tests was (besides time it took to open large assemblies)... try to replace an elbow with a tee.  In our investigations, the only program that did this simple test well, (or at all), was Inventor.  I complain a lot about functionality that is missing or outdated in Inventor Tube & Pipe, but I stand behind it as the best piping CAD system currently available.  

There's nothing wrong with wanting to be even better though, eh?  😉

[salariua]

Don't know about other software but we are doing process piping even though on all manuals and references it says that "It is not intended to be a process piping application". 

[cbenner]

Process piping is all we use it for:

[jeanchile]

"don't antagonize to much. Start working, it's far better experience to learn and discover this yourself."

Thank you Adrian, I appreciate the help. Unfortunately (fortunately?) my company has a strict software implementation study that needs to be completed prior to us rolling out software tools. I'm glad we have it, most of the time because it saves my company a ton of money to have one guy developing the procedures for this (and developing fixes for bugs) before everyone in the company starts using it.

I'm not sure what AD meant by not recommending that we use T&P for process piping but I assume they're talking about a large plant or something like it. We absolutely intend to use it for our process piping in the skids we do but we also intend to use it for the projects we do that are just piping at all of our oil & gas facilities. That is, of course, if we can get it to work the way we need. I seem to be struggling to get this module to work the way we need "soup to nuts". I'm hoping once my study is done I will have streamlined our process from initial routing all the way through to the weld mapping on the spool fabrication drawings.

I appreciate the help everyone. I'll keep plugging away. My next challenge is deciding whether to use the CC library to create my own parts or whether to just create all of pipe and fittings custom.

[salariua]

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@jeanchile wrote:
I'm not sure what AD meant by not recommending that we use T&P for process piping but I assume they're talking about a large plant or something like it.

I am sure they meant linking P&I D with 3D data and all the usual hassle.

I appreciate the help everyone. I'll keep plugging away. My next challenge is deciding whether to use the CC library to create my own parts or whether to just create all of pipe and fittings custom.

I would use CC, it's so easy to change size, rather than search replace from disk. Just out of curiosity, what other software are you considering?

[jeanchile]

Thanks Adrian, I'm really sorry for the late response. I got into another project that took me away from this for a bit and I'm just now getting back here.

We are not necessarily looking into another software package because of tube & pipe but there has been some investigation into another software package because of AD's stated goal of getting everything into the cloud. That's a deal killer for my company. During those investigations I've learned some interesting things about the other software packages out there is all. Certainly not saying one is better than the other but just some of the "I wish this worked the same way over here" kind of things.

I have a few more questions for you genius' when you have some more time:

1.) When I populate a route and IV creates all the part files, it says in Curtis' book that the files are saved to the standard CC part file location mapped in either the project or the application options. Does this mean that all the part files created by T&P are standard parts that are not editable afterwards? I need to be able to populate a route and then add project specific information to them that changes every time. If the flanges T&P creates cannot be edited after they are created this investigation is over.

2.) We don't use pipe "schedules" around here. Everything we do is using the decimal wall thickness. E.G. pipe is called out in the parts list as PIPE 6"SCH. 80 / XH / 0.432" W.T. but when we select it from our custom CC parts the keys are just the Nominal Diameter and Wall Thickness, not schedule or class description because it's the only property that exists for every pipe. Is this going to be a problem when we create all of our new pipe and fittings (i.e. does Inventor need us to use the schedule number somehow)?

3.) This is a weird question but... Has anyone ever considered just using frame generator to place all the pipes in there and then use the end treatment tools to adjust the lengths around the fittings? I know this is not going to be as efficient as using the T&P tools but depending upon the way this thing pans out, we may not be able to use T&P anyway.

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