Structural piping options without Routing

[laukejas]

Hi!

I am building a homemade ROV as a hobby. All designed in SOLIDWORKS. For structure, I want to use PVC pipes and fittings, which is a very common solution for homemade ROVs. I have an educational license on my home computer, so no add-ins, no Routing, which would probably be an obvious choice for this. Here are a few screenshots of what I did so far.

So, I'm wondering what the best strategy to model such a thing. The most obvious choice is multibody Weldments, which is how I did it right now (and not happy about it). 3D skeleton sketch for the lines, and then a custom profile for the PVC pipes. However, fittings are a total nightmare. I did them with Library Features, but you know how Library Features are Getting them to work in any orientation, select correct references, cut the correct bodies, and produce new bodies is an art of it's own. I spent at least 30 hours preparing the the Library Features for these elbows, T-joints, 45° joints, etc., and they still only work half of the time (and the other half, I have to manually repair each instance). As an added "bonus", Weldments sometimes get funky with Library Features - not grouping identical bodies, failing to produce correct lengths, or even outright not recognizing some pipe sections as Weldment members.
And if the fitting model changes... Oh boy, good luck fixing all these different Library Features.

I am attaching this .SLDPRT to this topic if you want to take a look at how I did it. The problems will be obvious and glaring. To add on top of that, Exploded Views don't work well with multibody parts - limited options compared to Assembly exploded views, can't be animated, etc.

I wonder what alternatives there are. If staying on the multibody approach, I suppose the frame could be done with Weldments, and the fittings could be done with Import -> Part. However, they would have to be positioned with Move/Copy feature, and we all know how much "fun" that is Then, trimming the pipes would also present a challenge. I suppose the fittings could have some trim planes that could also be imported, and then used for Weldment Trim/Extend. But that would create a lot of features.

Perhaps, alternatively, pipes could be done in a multibody part, fittings added in an assembly, and then part edited in context to use the cut planes of the fitting components for the Trim/Extend feature. Or maybe even Smart Components (have the fittings do the cutting).

I have not tried Structure Systems yet. Is it even worth investigating, would it provide any advantage to fittings problem?

I suppose I could also do such a frame as a Top-Down Assembly, meaning, creating a 3D skeleton sketch, and then a bunch of virtual components (each copying one line from the skeleton sketch, and then using Weldments), and the fittings could be Smart Components that trim these pipe components. When the final number of components is known, these virtual components could be saved to separate files. However, this wouldn't work for fittings that split a single pipe into multiple pipes, like these 45° joints in the pics above. I would have to know beforehand how many pipe sections I need in any particular location, and this would disrupt otherwise a very fluent workflow. Moreover, this approach wouldn't be very convenient for major modifications and re-design of the frame (compared to multibody Weldments), because then I would have to delete or repurpose these components, create new ones, deal with lots of lost references...

Do you have any comments on this? Perhaps there is a better solution than the ones I've tried? I know that this is a super simple project, so honestly it doesn't really matter that much, but I want to learn the best solution to this problem in general, so that it could be scaled and used on more complex projects, and suggested to customers, who might also find Routing to be an overly expensive overkill for their needs

Attaching the SW file for reference.

EDIT: I tried the Top-Down Assembly method as well (with Smart Components). Damn it is cumbersome (compared to multibody Weldment approach). Mirroring and patterning is really a headache, and requires trickery. For example, SW doesn't allow to mirror fittings if they are Smart Components... But if you turn them Lightweight, then you can mirror them. And for some reason, you can't mirror a Smart Feature inside a part (for example, to get an identical trim on the other side of the pipe - you have to cut the pipe in half with Cut With Surface, and then use Mirror Bodies. All of this is doable, but really time consuming, and would require lots of re-work if pipe structure would be changed, like one of the member split into two, etc.
Check out the attached Frame.zip for this attempt.

Really looking forward to any suggestions on how to do this better in Assembly mode

[gupta9665]

You can develop individual parts with configurations,smart features and mate references. This way you can create the required assembly much faster and reuse most of the parts.

[laukejas]

You can develop individual parts with configurations,smart features and mate references. This way you can create the required assembly much faster and reuse most of the parts.

How exactly would I set it up with configurations? I want to control everything through that main skeleton (layout) sketch, it should be driving the lengths and positions of each pipe segment.

[Tom G]

@laukejas, you're making what I make all the time, to some extent. I have well developed assembly methods that are stable and do not require Routing. I don't have time today to elaborate well, but I will gather some images to discuss over the next few days when I have a long weekend. I've been meaning to explain more here (@JuTu is interested as well), and you've shown your efforts into learning this.

Super brief summary of what I'd like to explain:
Prepare components with sketches upon which to place weldment 3DSketch endpoints
Arrange in assembly
Weldment pipe as virtual component in assembly context
Strengths in fabrication / purchasing results

[laukejas]

@laukejas, you're making what I make all the time, to some extent. I have well developed assembly methods that are stable and do not require Routing. I don't have time today to elaborate well, but I will gather some images to discuss over the next few days when I have a long weekend. I've been meaning to explain more here (@JuTu is interested as well), and you've shown your efforts into learning this.

Super brief summary of what I'd like to explain:
Prepare components with sketches upon which to place weldment 3DSketch endpoints
Arrange in assembly
Weldment pipe as virtual component in assembly context
Strengths in fabrication / purchasing results

That sounds awesome. I am waiting for that info

[Lucas]

That's a cool project, congratz for it.

In my option using Library Features is the hard way to do it. You only need to create the Weldment profile for it, not all the parts.

How I would do it:
Since it's too many bodies I prefer to work in assembly, I would create one part for the weldment - grouping closed loops or parallels like this:

Then make the joints parts separately and insert them in the assembly, positioning them in a way to use Mirror feature.

Then go back to the weldment part, create planes and use Split feature to cut them. (it's easier to see or change the cut later)

The multibody way I would use the Intersect feature:



Multibody is better if you want to use Boolean operations (Combine, Intersect, Indent and Split), but it's harder to position the parts and the file becomes slower.
In assembly the only Boolean operation available is the Join feature which merge the parts, it's not possible to substract or intersect (would be super convenient)...

[Lucas]

I have not tried Structure Systems yet. Is it even worth investigating, would it provide any advantage to fittings problem?

Structure System is able to create everything with box selection, so it's faster than Structure Member in that way.

Additionally another option is add construction geometry in the 3DSketch and trim the unwanted part, this way you are able to edit it later. Although 3DSketch has some trouble depending on the way you set relations and stuff, sometimes it jams.

[laukejas]

That's a cool project, congratz for it.

In my option using Library Features is the hard way to do it. You only need to create the Weldment profile for it, not all the parts.

How I would do it:
Since it's too many bodies I prefer to work in assembly, I would create one part for the weldment - grouping closed loops or parallels like this:
ezgif.com-gif-maker.gif

Then make the joints parts separately and insert them in the assembly, positioning them in a way to use Mirror feature.

Then go back to the weldment part, create planes and use Split feature to cut them. (it's easier to see or change the cut later)

The multibody way I would use the Intersect feature:

Multibody is better if you want to use Boolean operations (Combine, Intersect, Indent and Split), but it's harder to position the parts and the file becomes slower.
In assembly the only Boolean operation available is the Join feature which merge the parts, it's not possible to substract or intersect (would be super convenient)...

Thank you for taking the time to try this out. There are missing files in the Assembly you attached, could you please upload a full Pack&Go, so that I can properly understand how you made this?

[Lucas]

Thank you for taking the time to try this out. There are missing files in the Assembly you attached, could you please upload a full Pack&Go, so that I can properly understand how you made this?

I can't get them now. They are the same files you send, I just modified the assembly and saved with another name, if you paste it on the same folder will work.

Basically I just created a new virtual part, made a 3DSketch and Convert Entities from yours, then made the Weldments, two Planes and used the Split feature. I just did a quick demonstration to show the tools to you ^^

[JuTu]

Hi!

Thanks @Tom G for the hint!

Yes, interesting project!

@laukejas, are you sure your educational license doesn't include those add-ins? What if they are just not activated in SW?

Well, anyway. I dont have enough experience for configurable assemblies or parts so that goes outta the window straightaway.

If all those elbows and other fittings are standard off-the-self parts, I probably would tackle this puzzle in assembly mode.
Prepare part models for elbows with point or other sketch entity that you can use as pipe start/end point. You could create a master sketch within the assembly and with in-context edit convert all those sketch entities to the part where the lines would be converted to weldments.

This is a rather intriguing problem!

[Tom G]

That sounds awesome. I am waiting for that info

Sorry to keep you waiting. I ended up travelling on short notice this weekend, but all is well. Will elaborate.

[Tom G]

Words needed. In the meantime, here's worth a few thousand. 6/10/22 Edit: More words added. I think it needs an intro and conclusion still.

Three Tees:
Each fitting part has a Weldment 3DSketch which converts entities upon the inner edge of the pipe seat. The colors differentiate plastic pipe, metal pipe, and metal tubing. The circle or Arc is not the valuable asset in these sketches. The valued reference is only the center point of that arc or circle. The first two parts contain very many configurations for sizes, materials, ratings, and connection types. The third part is a single configuration purchased product. Each Tee is oriented the same, with its through axis on the X Axis and the branch axis on the Y Axis. Each one has reference entities of Axes and Planes, named exactly the same where its application matches (i.e., pipe or tube). All reference entities (except the Origin for some reason) are available in an assembly when the component is lightweight. The 3DSketch is only available when the component is resolved. This detailed attention to components is critical for later processes here to function robustly and interchangeably. This component definition is also a parallel process to the requirements of the Routing Library Import Wizard, but it is in my own manner for my own multipurposes. The 3D Sketch entirely replaces RPoints which are used in Routing, and carry no associative size variable.

(added)
Due to the exactly named and defined reference planes across all similar objects, I am able to handle two objectives of Routing with little additional effort. Because all mates are ideally defined exclusively between reference entities of the components, I am able to dynamically replace all plastic tees with compression tees, or socketweld metal tees, for example. Sometimes I change the size of a pipe train by exchanging a single-configuration component with another single-configuration component. Other times, I can select a different size from within a multi-configuration component. When I change size by component configuration, the secondary derived pipe or tube does not require its sketch relations to be reassigned.

(added)
Here is the one hang-up that does not happen automatically. When changing from one component to another, the sketch point of one component does not have its relation updated to the similar sketch point in the new component. Therefore, after the component is replaced, Errors will pop up within the 3DSketch of the virtual Pipe/Tube component. All that is needed to resolve this is to use Display / Delete Relations tool within the pipe/tube 3DSketch to delete dangling Relations, then reattach the endpoints of the sketch to the similar sketches in the new component. Then it can rebuild and resolve its errors.

One compression adapter:
You can see here that the manufacturer-provided imported geometry does not have a circle at its seat. Sometimes components have a face split along its entire length. This matters nothing to me, because the Arc in this sketch has the same center point to refer to as a circle would. However, if the imported geometry is flawed so that it is neither an Arc nor a Circle, then it will not have a center point to go with the converted edge. In these rare cases, I may define two equal colinear lines across the seat and On Plane to a primary reference plane, in order to create an actual point at the correct location. End points work just as well as center points. Midpoints are a pain in the assumption.

Arrange your assembly with mates between adjacent fittings exactly as using Axis coincident to Axis, FacePlane distant from FacePlane, and a primary reference plane parallel to something. Elbows sometimes need the same constraints, but sometimes only two Axis-Coincident mates will suffice. Applying all mates in all manners will overdefine the assembly. If applicable, I may define a Global Variable in the assembly to represent visual pipe length as the default value for face distant from face mates, with other values applied as desired, such as where a support or hardware will land upon the pipe. I use 2" spacing on socketweld, 3/4" on solventweld, 1/2" on compression, and no GV for threaded.

(added)
For Skeleton Sketch Part method, I utilize a Skeleton Part comprised mainly of Planes. This is because my SSP method primarily does not derive features or bodies, but rather it controls assembly mates of unchanging library components. The secondary derived Pipe or Tube is the dynamic feature, related to the Weldment sketches of the components in a 3D Sketch, and then populated with Structural Member profiles.

(added)
Separately, these planes also accept relations for derived bodies within the actual support structure comprised of Structural Member features. This is tertiary in my design, adapting to the defined planes in the SSP and in the process following the primary assembly of components connected by secondary pipe or tube.

This is one SSP that I use.

(added)
If sketches are shown in my assembly, all resolved fittings, valves, and connection entities have their Weldment 3DSketch shown. Here, I show the exterior of a shelter enclosure which contains a CPVC solventweld system in the corner, and a metal socketweld system next to it. The color-coded objects (not shown, structural supports' sketches get colored bright or dark green) are entirely unnecessary, but it can be helpful to determine which types of objects are where, especially where they are both present, such as the assembly image above which shows a metal piping system with a compression tubing vent connected to a vent of the calibration column.

(added)
The virtual pipe/tube components made up of Structural Members are very stable, especially when they are compartmentalized by subassemblies within a Large Assembly. Below you also see evidence of several subassemblies: the plastic system, the metal system, the building itself, the structure that it all rests upon, and the electrical items (and/or conduit, as applicable). Once the entire assembly reaches the threshold of Large Assembly Mode, only the subassemblies which are relevant to be worked upon are resolved, where the rest of it remains lightweight.

[laukejas]

Hi!

Thanks @Tom G for the hint!

Yes, interesting project!

@laukejas, are you sure your educational license doesn't include those add-ins? What if they are just not activated in SW?

Well, anyway. I dont have enough experience for configurable assemblies or parts so that goes outta the window straightaway.

If all those elbows and other fittings are standard off-the-self parts, I probably would tackle this puzzle in assembly mode.
Prepare part models for elbows with point or other sketch entity that you can use as pipe start/end point. You could create a master sketch within the assembly and with in-context edit convert all those sketch entities to the part where the lines would be converted to weldments.

This is a rather intriguing problem!

Yeah, my license definitely doesn't include any add-ins. Thanks for that suggestion. I did try the assembly method with a master sketch. Problem is, creating individual parts for each pipe segment manually is very time-consuming, especially because there are lots of very short pipe segments. It is difficult to determine how many segments there will be after the joints finish cutting and trimming them.

For example, imagine I have a straight pipe segment running from one elbow to another. And then I decide that I want to place a T-joint in the middle of that pipe. Meaning, this pipe now becomes two pipes. This is a nightmare in assembly mode. I now have to create additional virtual component, save it, fix broken mate references at least on one end (with the elbow)... Weldment approach causes no problems here - it just splits a pipe body in two, and that's it, nothing is broken. But like I said, Weldments are limited in other ways, so I'm looking on how to solve this kind of a problem easily in Assembly mode.

Words needed. In the meantime, here's worth a few thousand.

Thank you for these images, Tom. But could you please elaborate a bit more about how your assembly is structured? I think I understand how the joint parts are built, but I am unsure what the pipes are. Is each pipe an individual body? Or is it multibody Weldment that is trimmed by these joint parts?

Like I said, I want to find an easy way to build this purely in Assembly mode (no multibody parts), but creating these individual parts is a headache, because it takes so much time to create each pipe segment, and like I wrote above, often I do not know if a particular pipe will be continuous or split into two by some joint. I suppose I could place joints first, mating them to the assembly layout / master sketch, and filling in pipes afterwards, but that is a very non-intuitive way to design stuff like this.

[Tom G]

For your weldment profiles, you don't need custom profiles. You should be able to retrieve a whole package of standard profiles here:

You will find many sizes of SCH.40 and SCH.80 pipe there, under Pipe (Structural).

For your case - I am unclear what you want to do with this.
You say you are building this. Are you 3D printing components? Are you purchasing components? Are you 3D printing the entire assembly? Are you gluing things together with pvc cement (solventweld)? Or did you mean that you are building this as a virtual project to produce a CAD design as an exercise?
Far more importantly here, what are you doing with the design data? Are you simulating is performance? Are you measuring internal volume for buoyance? Are you producing assembly drawings? Are you producing a Bill of Materials? Are you exporting 3D PDFs? Are you making pretty images (such as the exploded view) for the purpose of learning, or for purposed documentation?

If you desire to model a single pipe nipple as a component, that's doable but entirely cumbersome. I did the same thing when I first began. It is unnecessary. I still have some unused Nipple.SLDPRT lingering in my design library, a remnant from those first attempts. Pretty soon I found weldments. Your intuition is just as wrong as mine was, and assembly is the strongest tool for putting things where they belong and then stringing the pipe upon it afterward. (In my practice, items come first, pipe second, and structure third, which is exactly the opposite of its manufacturing process.) Design doesn't have to be a Lego set where the thing on bottom comes first and the second piece needs added before the third or fourth piece can be added. That is the nature of physical reality. Design is not yet reality but it can guide and inform reality.

Let me clarify a distinction. Methods need to inform and and assist what you want from it. So what do you want from it?

Explicit example: I do not even end pipes where pipes end unless it's made of unobtainium alloy. I don't care one bit about pretty representations, exploded views, sections, or simulation. I do care about representing a singular unique thing clearly on a drawing for customer approval, and then driving the data into business practices of purchasing, receiving, fabrication, assembly, inspection, testing, and shipping. Therefore, where I show you a pipe from a flange through a valve, through a backpressure valve, through a tee, through a union and so on, it is one continuous body made with a weldment feature in a fixed virtual part, driven by a 3d sketch within that virtual part which relates only to its endpoints upon the objects at the end of straight runs of pipe. All of the multiple bodies within my virtual weldment pipe part are produced with a single weldment profile - which means it is one single size. This allows me to measure total length of all sketch segments in its 3DSketch, apply that value into a custom property, push that value into a BOM, where it represents one single size of pipe / tube and its length, which is sorted and similar items totaled and exported to a static Excel document. The extra length rounds up the quantity which I instruct to purchase, which is then rounded up to purchased 20 foot increments anyway. Unused pipe sits on a stock rack, and the unique item is produced once and not optimized for mass production.

This is why I emphasize what you want from it. If you desire 100% single body parts for whatever purposes you require, then go ahead and do that. It is not the easiest way, but there is nothing stopping you from overcomplicating your arrangement. Even if you desire alternative methods, I will elaborate here on my methods among my images.

[laukejas]

For your weldment profiles, you don't need custom profiles. You should be able to retrieve a whole package of standard profiles here:
GetWeldmentProfiles.JPG
You will find many sizes of SCH.40 and SCH.80 pipe there, under Pipe (Structural).

For your case - I am unclear what you want to do with this.
You say you are building this. Are you 3D printing components? Are you purchasing components? Are you 3D printing the entire assembly? Are you gluing things together with pvc cement (solventweld)? Or did you mean that you are building this as a virtual project to produce a CAD design as an exercise?
Far more importantly here, what are you doing with the design data? Are you simulating is performance? Are you measuring internal volume for buoyance? Are you producing assembly drawings? Are you producing a Bill of Materials? Are you exporting 3D PDFs? Are you making pretty images (such as the exploded view) for the purpose of learning, or for purposed documentation?

If you desire to model a single pipe nipple as a component, that's doable but entirely cumbersome. I did the same thing when I first began. It is unnecessary. I still have some unused Nipple.SLDPRT lingering in my design library, a remnant from those first attempts. Pretty soon I found weldments. Your intuition is just as wrong as mine was, and assembly is the strongest tool for putting things where they belong and then stringing the pipe upon it afterward. (In my practice, items come first, pipe second, and structure third, which is exactly the opposite of its manufacturing process.) Design doesn't have to be a Lego set where the thing on bottom comes first and the second piece needs added before the third or fourth piece can be added. That is the nature of physical reality. Design is not yet reality but it can guide and inform reality.

Let me clarify a distinction. Methods need to inform and and assist what you want from it. So what do you want from it?

Explicit example: I do not even end pipes where pipes end unless it's made of unobtainium alloy. I don't care one bit about pretty representations, exploded views, sections, or simulation. I do care about representing a singular unique thing clearly on a drawing for customer approval, and then driving the data into business practices of purchasing, receiving, fabrication, assembly, inspection, testing, and shipping. Therefore, where I show you a pipe from a flange through a valve, through a backpressure valve, through a tee, through a union and so on, it is one continuous body made with a weldment feature in a fixed virtual part, driven by a 3d sketch within that virtual part which relates only to its endpoints upon the objects at the end of straight runs of pipe. All of the multiple bodies within my virtual weldment pipe part are produced with a single weldment profile - which means it is one single size. This allows me to measure total length of all sketch segments in its 3DSketch, apply that value into a custom property, push that value into a BOM, where it represents one single size of pipe / tube and its length, which is sorted and similar items totaled and exported to a static Excel document. The extra length rounds up the quantity which I instruct to purchase, which is then rounded up to purchased 20 foot increments anyway. Unused pipe sits on a stock rack, and the unique item is produced once and not optimized for mass production.

This is why I emphasize what you want from it. If you desire 100% single body parts for whatever purposes you require, then go ahead and do that. It is not the easiest way, but there is nothing stopping you from overcomplicating your arrangement. Even if you desire alternative methods, I will elaborate here on my methods among my images.

Sorry for a late reply, forum didn't send me a notification You raised some valid points here. Let me answer what you asked, and then list the requirements. Like I wrote, this particular frame build is just for a hobby, but I am also trying to learn new ways to tackle piping design in SOLIDWORKS so that I could suggest it to our clients at work, which might be doing this on a far larger scale and complexity. For this specific build, I am going to cut the PVC pipes to length from a cut list, and then glue them with PVC cement to these joints, elbows, etc. Some will remain unglued and will probably be secured with screws or bolts to allow for partial disassembly. There will be 3D-printed parts in this project, but not in this frame - all components here are purchased.

So, what I need from this is:
1. Quick, easy and intuitive modeling of frames like this, especially when I need to make major changes, like deciding to split a certain pipe into two with a T-joint in the middle, making a mirrored section independent so that I can make some changes there, adding in new pipe sections, swapping one kind of joint for another, etc.
2. On the manufacturing output, I only need a cut list with accurate lengths of pipe segments. BOM too, but not that important (because the number of required joints is already obvious).
3. Measuring volumes is required, but I already figured that bit out, both in weldment and in assembly modelling approaches.
4. I also need an animation of the exploded view in the top-level assembly, including that frame, for demonstration purposes. This is a limiting factor, as currently SOLIDWORKS can't do exploded animations of multibody parts. And the exploded views are pretty buggy in parts anyway.

[Tom G]

Bump, extra explanations of provided images added to post above. Once finished, I will compile it into one post and repost it into the Best Tips and Tricks thread.