Can we create construction body in Solid Works? Is there a concept of Construction body and Designed body in Solid Works?
Can you explain what you mean by "construction body"? And this Question has been marked as Answered. You might get more responses if you change that.
There is not a definition for a Construction Body in SOLIDWORKS, however that does not mean you cannot create Construction Bodies. You would be required to manage the difference between your construction and design bodies. Manipulation of the bodies would be done in the Feature Tree under Solid Bodies where you have the ability to assign names to bodies and make those bodies visible or not. When creating the extrudes, lofts, revolves, etc. you would need to uncheck merge result if your new feature intersects both the design and construction body; then you would need to use the Combine feature to add like bodies together (design bodies to design bodies, etc.).
The best way to get a feel for what Solidworks can do for the new user is to do the tutorials:
Construction bodies are bodies which are not considered in drawings or mass properties.
Thanks for the info.
Does non merged body is considered while calculating the mass properties?
To manage Mass Properties you can create a "Construction Body" Material with zero density and assign it to the Construction Body(s).
How to make it unanswered?
Jadhav Vaibhav wrote: Hi,Construction bodies are bodies which are not considered in drawings or mass properties.
Jadhav Vaibhav wrote:
It's easy enough to exclude bodies in drawing views (see #15 at Frequently Asked Forum Questions), and for Mass Properties on the Evaluate toolbar in the Part you can choose which bodies to include. If you want Mass Properties of selected bodies in a Drawing you can use the Delete Body feature to delete bodies that are no longer needed.
There are always many ways to do the same thing within SOLIDWORKS. The way you do things may have differing effects downstream in design and other processes. The reason I suggested using the Solid Bodies in this manner is to allow the continued use of the "Construction Bodies" within Assemblies, and other processes such as CMM Fixturing. In the past I have used "Construction Bodies" as Fixtures within a part file and those bodies were used later in CMM setup as keep-out areas.
Jadhav Vaibhav wrote: How to make it unanswered?
I just checked. It's a little more complicated than I thought, but not too bad. Mark one of the replies as the correct answer, then Unmark it as Correct in the same place.
You can model with surfaces which have no mass. To exclude items from drawings and a BOM you can check that preference in properties of items in the feature tree.
The other option is to use John Stoltzfus's skeleton sketch method, which is kind of like using a construction body, but in a part specifically made as ONLY a construction body/sketch which all other parts reference in the main assembly.
This is my understanding of what you're trying to accomplish.
So you want to use a part/reference body to design around but you don't want that body to affect the newly designed assembly in ways such as mass and at a BOM level. I have used assembly/parts to design around and didn't want them to show at the drawing level and also to not populate on a BOM and since we display the mass of parts and assemblies on our drawings it couldn't affect that either. So i would turn the reference body into and "ENVELOPE" part which can be done through the "Component Properties", when you check the envelope box by default also checks "EXCLUDE FROM BOM". See how it changes the icon of the part file in you tree.
This is a nice feature but I have noticed that it tends to make your assembly really slow and become a resource hog (that's what I have noticed, may not be for all). So I tend to leave it "normal" until getting to the drawing level where I don't want to see it.
Hope this helps otherwise thanks for reading!!
I agree with this method and was about to suggest it before I read it.
I always thought the word "Envelope" made it sound like something different. Construction Body sounds like a good alternate.
Very cool feature.....I never experimented with it!
Thanks Dennis Schuette!
Edit: This will help a lot when I am designing fixtures! I always put the CAD model of the machine in and then have to play with suppression/Exclude from BOM..... This is awesome.
2015 SOLIDWORKS Help - Assembly Envelopes
Envelope is a common engineering term.
ICD's (Interface control drawing's), ID's (Interface drawing's), and many others control suitable definition.
"Envelope" is pretty much what anyone who works specifically in TOP-down design starts with.
Instead of using a body, I usually just use sketches for reference to parts that aren't really there, or are actually parts of a different assembly or mount. Maybe even use common ones as their own part.
Here is an example of a part with a 3D sketch that I use when I'm putting parts inside a box, or mounting parts outside and through said box, and that box has a liner or something that gives it thickness. This 'part' can either be used as the seed model or be inserted into an assembly. Then it's just a matter of attaching features to the sketch lines, and/or making reference planes in the part and attaching/mating other parts to those.
I have used solidedge with construction bodies for many years and it is a very useful feature and i know exactly what you want to do in solidworks however there is no real feature in solidworks that functions like construction bodies. The envelope method is not really the same thing and it is in the context of an assembly file not a part file.
A construction body is a externally referenced part within the context of a part file, not an assembly, and the construction body is a phantom body that can be only referenced to create in context part around it. The construction bodies has no other properties other than its geometry and it can be turned off and on in the part file. The design body can then be inserted into a lager assembly as an individual part. This is useful because most parts usually only reference one other part in a greater assembly. However when you design in context parts in a solid works assembly if references the part within the greater assembly file. Construction bodies is a good way to keep this simple and allow greater flexibility.
The closet method in this thread that acts like a construction body is the geometry sketch that individual parts can reference but not each other.
If a derived parts inserted into part files could be converted into phantom bodies that could be hidden, excluded from BOMs, part properties etc that would be a construction body. But derived parts in part files can only be deleted and once deleted you can no longer reference the part.
I use a similar method of creating construction bodies around which I create my final design. I do this in a single part file as a multi body part. I have two kinds of construction bodies: Layout and Obstructions. The layout consists of the pipes, fittings, valves, etc,... with which we are working. Obstructions are other pipes, fittings, valves, walls, etc,... that are around the layout and create space constraints for the hardware we design that attaches to the layout hardware. When I start a new part file, the first thing I do is create the Layout bodies. I then go to the Bodies folder and select ALL of the various bodies that are part of my Layout. I right click and pick "Add to New Folder". I then name that folder "Layout". I have created a custom material called Layout. It has a density of .00000000001 lbs/cu.in., effectively zero. Solidworks won't actually let you enter zero for the density. I also set a specific color for the Layout material so that it is quickly identified in the model space. The next thing I do is create the bodies that represent any obstructions. I have a material for obstructions with a near zero density and custom color as well. Once all the obstruction bodies are created, I do the "Add to New Folder" with them and call that "Obstructions". The nice thing about the folders is that you can control the visibility of the bodies at the folder level rather than having to select all the bodies individually. Of course, if needed, it can still be done on a body by body basis.
Now, when I start creating the actual design hardware, it has a normal material with regular properties. The design hardware usually consists of multiple bodies as well so I group them as needed in subfolders of the Bodies folder. My only gripe is that I wish you could select bodies by folder for operations like the Mass Properties command or when deciding what to include in a drawing view. I am using SW 2014 and it still requires me to open the folders and actually select the bodies or select them in the model space. But if I need the mass for a given part of the design, I can still open those folders and select all the bodies for that folder if there are a lot of bodies, or if there are only a few, I will select them in the model space. I could split all the various bodies out to new part files and then reassemble it all in an assembly file, but for what we do, that just adds a LOT more files and time. The way I do it now, I have one part file and one drawing file, which makes house keeping a LOT easier! The only down side is that when I do my drawings, the mass is not pulled in automatically for those jobs that have numerous bodies. For these, I just use the Mass Properties command and then manually edit the automatic figure in the drawing with the mass for each piece of the design as needed.
See Envelopes in the Help Section.
I didn't read through this whole thing as there were too many words, but I didn't see the words
I use them all the time as reference geometry.
Edit: I see that Ben mentioned the use of surface bodies.
I believe the envelope option is only available when you are in an assembly file?
For the work I do I would have to have a separate part file for my layout, obstructions, and then each piece of the hardware actually being designed. That adds a LOT of extra steps and files for me. The work we do is very time sensitive (like they want a design back in a matter of hours from the time they call in the information). Anything that cuts down on the number of steps from beginning to end is critical for us. By doing the multi body part file that is already essentially an assembly file in function, we can do every thing in one place without having to move around through various files. We are not doing super complicated stuff with tons of different parts, assemblies, sub assemblies, etc... So our case might be a bit unique. I can totally see how the envelope feature would be very useful in more complicated stuff. On rare occasions we do have projects where the more typical multiple parts with assembly files process will be desirable. Prior to today I was unaware of the envelopes option, so thanks!
You are correct. Only in assemblies. It would be nice for part features. You can still do some of the basics of envelopes in a part file. Change the transparency of the body. Add a noticeable color to it. If weight is important to you, make a zero weight (.00000001) material special for the application. This of course as others have suggested, would be a multi body solid not merged with anything that is important to you. So this could work just fine. If you really want to use surface bodies you can too. You can always make a surface body from a solid by selecting all the faces of the solid and offsetting a surface a zero distance. Then go back and delete the body with the delete body command. I can't necessarily come up with a great reason why. Just giving the suggestion. Hope this helps.
One can also import sketches into a part and use those. Even fully 3D sketches can be copied from another SW file into a part.
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