Does Solidworks have "construction" bodies

SOLIDWORKS How To Questions
1

In the past I have used multiple bodies in a part file, not as multiple parts but as tool bodies or other “helper” geometry. Instead of trying to do everything as one body sometimes the feature tree can be much simpler by just using another body and doing a union or subtract, whatever. Sometimes create the body to create needed guide curves (this could probably be done in a 3D sketch nowadays…)

Anyway, the question is, does Solidworks have a way to mark a body as “construction” meaning it has no material, no mass, not part of physical properties calculations all that kind of thing. I used this a lot in Solid Edge and I’m not seeing the option in Solidworks, kind of missing it.

Here’s what it looked like in the “Path Finder” in Solid Edge:
image.png
Another post about weldments and trimming bodies is a good example and since it was mentioned to set the material of the tool/trimming body to near 0.0 density I’m guessing Solidworks does not support this:
https://www.cadforum.net/viewtopic.php?p=3882#p3882

2

I believe what you are refering to would be envelopes

https://cadbooster.com/using-envelopes-as-reference-models/

3

Yeah, envelopes may be a way. Another is to just use the SSP method. The driving part doesn’t have to be composed of just sketches, you can use surfaces, solids, or whatever you want in the driving part. Then just exclude the driving part from the BOM and keep it’s material unassigned, and it won’t affect the quantities or mass.

4

envelopes are just for assemblies.

generally you would delete the extra bodies at/near the end of the tree to remove it from part

5

I’ve occasionally done something similar, usually to drive a 3d sketch. I typically use the “Delete Bodies” feature when I’m finished referencing it. That gets rid of it, but keeps all references intact.

Edit: I see Jeremy Feist beat me to it.

6

I’m sorry, I don’t understand SSP here. You mention “the driving part” what do you mean by part in that context? Is it another file in an assembly that contains the desired part and all the tool bodies? I’m confused because just a sketch, line, surface, etc in a part file is just geometry.

What does excluding from BOM mean? I’m not familiar with a part file having a BOM.

7

Delete bodies does work. Make certain to not merge bodies in features, or to control which bodies are merged. Simply beginning a weldment feature, even if you will not use it, does flag any subsequent features to be non-merging by default.

There’s more than one way to perform this. You can also use the assembly tools. Build the real part virtually, referencing the envelope component. I make sure to control invisibility of the envelope part once completed.

8

Maybe I’m not understanding what your attempting to do or why, but why can’t you just create the body you want to subtract as another part, insert it into the part you want to modify and combine? If you want to change the inserted body you just go and change the inserted part. If you’re all done and will never have to do any changes to that again break the external references.

9

So I tried to reply to this earlier, but the forum blew up.

Anyway, I used what you could call “construction bodies” all the time.

Basically, it is a just a regular body (either modeled in, or inserted), then I change the Body Display for that body to wire frame.
image.png
Then, once my project is done, I run a Delete Body Function and remove it (its a step in the history tree, so it just doesn’t show up in the final product).

In an assembly environment, there are “construction parts/sub assemblies” and Solidworks calls them Envelope components.

10

It sounds like the answer is:

No, Solidworks doesn’t have a way to segregate bodies for construction vs design but the consensus is to just delete these bodies at the end. I marked the first response with this suggestion as the best answer, although others added helpful bits as well.

I think this sounds good to me. It is nice the Solidworks doesn’t have the concept of “active body” like Solid Edge does. Each feature can be a new body or merged with any existing. In Edge that’s not the case.

Thank you all.

11

I use surface bodies for this purpose.

Unfortunately there is no nice way to create them from solids out the box.

There is an amazing trick invented by zxys001 that works.

Subtract the body from an encompassing sphere and then use delete face on the sphere face.

They are so useful I added the functionality to my Add In

I call it going ghost..
image.png
image.png
artem also has this feature available, but I’m not sure where it is now that the old forum is gone sorry.

12

I think you got it. Keep a few things in mind though

  • that’s another file to manage
  • these parts live “forever” and will likely need to be edited in the future in a way that avoids removing geometry that might have mates or annotations attached to them. So there is no “just delete the feature and recreate it.” actions. Using mulit-body workflows SOMETIMES makes for a more stable feature tree, in my experience.
  • the file will be edited by various users so they will need to understand the purpose of the other files and make sure they check that file out and it moves through the PDM workflow states, unless we put it in a library category that doesn’t have revision control but would still need to be checked out…

It just gets very messy to have data in several files that could all be in one. Consider the concept of data encapsulation where all the stuff needed to define a tangible, physical object in a model can all live in that part file. Unless a portion of that data is not solely controlled by or exclusive to that object, it should be in one file. Just my opinion, in my mind Object Oriented programming concepts tend to find applications outside of programming.

13

As is usually the case “All depends on how you plan on using it” :smiley:

If it’s a part with a long life that will be used in multiple places, revised and so on, probably not the best approach. But if it’s a case of a one off that likely won’t be revised after it’s released then you can just break the links and have one part.

14

Yes!! UU

edit.. we are programming

15

I’ve sat down to respond to this thread 3 or 4 times now, and I’ve lost my response every time because I got distracted by other stuff.

Anyway, If I’m not mistaken, Solid Edge refers to surfaces as “constructions”. So “construction bodies” don’t have the meaning you think they have. They are just referring to surface bodies.

Solid Edge has other odd designations for bodies:

  • the user decides when to call whatever you’re building a “new” body
  • a single “body” can contain several distinct volumes
  • in addition to “Design Body”, there are also designations such as active and inactive bodies.

I would like to see a chart of all of the states of bodies in Solid Edge. I was there when they came up with a lot of this, and they did talk to me a bit about how bodies work in SW, but to be honest, every time I need to work with bodies, I have to go back and figure all of this out again.

16

I reread this and I realized I misread it the first time. I thought bodies could be “Design” or “Construction”
image.png

17

You’re right, I was mistaken when I wrote that. But I still can’t say that I completely get this. Surfaces in Solid Edge are by default “constructions” or “construction bodies”. And solids can be set to construction, but they are by default “design bodies”. Surfaces as far as I can figure out cannot be design bodies.

I think construction vs design means it gets counted in the part mass, and some other things. Rough equivalent in SW is a combination of surface bodies and envelopes (except envelopes can only be parts in an assembly, not bodies in a part, but its a similar concept). I’m writing this out mainly to make sure what I’m saying makes sense, which I’m not really sure about.

“Activated” vs “Inactive” I think allows you to assign which bodies will be affected by new features. I think this only applies to solids, not to surfaces, and the SW equivalent is the Feature Scope selection box within each feature PropertyManager.

And then beyond that is “Activated Assembly Body” which means that body is shown in an assembly, and anything that is not an “activated assembly body” is not shown when the part is shown in an assembly. Whew. Is that right? As far as I can tell, only design bodies can be activated assembly bodies, but there is a way to show a surface in an assembly, I just can’t remember what it is.

Ah - ok, a little google search, and I remember. There is a setting in Options>Settings>Assemblies for showing construction bodies if a part has no design bodies. And then there is another option. If you right click in the assembly on the occurrence (I think that’s the right SE word instead of SWs instance or component), You get a list of stuff to show, “Surfaces” being one of them. Interestingly, when I do that with my experiment part, even the solid part turned to a construction body is shown, in addition to the surface. So that option really should read “Construction Bodies” instead of “Surfaces”.

I think all of this could have been simplified.

This is all in addition to the user determining when a new body is created, there is no requirement that a “body” have a “single contiguous volume”. And it seems SE doesn’t really consider surfaces to be “bodies”, they are “constructions”.

In the image, the two gray solids are both a single body. The blue are both constructions, even though one is surface and one is solid.
image.png
Calling Imics13 to verify or correct.

Describing SW bodies to a noob user is much easier than describing SE bodies, at least to me. I’ve never seen it all laid out in one explanation that makes sense. I just get little pieces of it at a time, and so I’ve never connected it all until now. Does this seem more complex than it needs to be to anyone else? Does anyone have a good way of explaining it? (Again, looking at Imics13 )

18

ok. that makes more sense. I too understood that for SE “Construction Bodies” meant they would not be included in physical properties and weren’t shown by default on the drawing. I concluded from the comments that the way to do this in SW is to delete the body at bottom of the tree or when done with it. Okay.
edit: I reread your post, again, and I think if I had not used SE it still would not make sense. I think the layout may be from the addition of functions though the years. I don’t know when SE added it but I know at one point they did not allow non-manifold bodies. Perhaps the “Active Body” concept was a solution to the “which body are we working on now?” question where as Inventor and Solidworks all the bodies are active and they ask, “Which body would you like this feature to act on?” I couldn’t find where SW has the notion of Construction Bodies, all the bodies are available for nearly any feature all the time, if you don’t want bodies to show on drawings or included in BOM or physical properties then delete them when you’re through. I cannot remember what Inventor had for construction vs design bodies.

Activated body in SE sucked in my opinion, it was not clean way to select which body to do operations on. For some reason I was thinking that I could only have one body active at a time. Solidworks and Inventor do much better, all of the bodies are always available for operations and you select which bodies to act on or merge in the feature you’re doing.

19

It’s kind of a moot point if you’re going to use synch edits in assemblies and your parts always have only one body.

I have considerably soured on SWX multibody modelling recently. They have no “good” workflow for exporting them. If you seriously believe they do, try using a gauge table… ~~~~ My theory? They purposely have four ways of splitting up part files (Save Bodies, Split, Insert Part, Insert into New Part) so the techs can just recommend a different, but equally flawed, method to the unsuspecting user.

20

I’ve always avoided multibody sheet metal just because it seemed like an awful lot to control in a single file. Splitting up the parts is a small price to pay for the compartmentalization (is that a word?) of all that info.

~~~~ > My theory? They purposely have four ways of splitting up part files (Save Bodies, Split, Insert Part, Insert into New Part) so the techs can just recommend a different, but equally flawed, method to the unsuspecting user.

My theory was that they had 4 different people who designed the functions, and they couldn’t work together, and once they made one, they had to leave it in for legacy reasons. They should have just combined all of them into a single feature with options for how you wanted to handle the data. The 4 headed beast is tough to explain to people. On my Episodes pay site, this is how I explained it in a chart:
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