Solidworks: Correct Workflow For Modeling An Assembly?

Hi, I’m fairly new to SW and would like to know the best way to model a product comprised of various parts. I’m modeling without drawings so it’s a bit difficult to model each part in a separate file and for them to perfectly match up when assembled.

What I’ve been thinking is to model the basic block form as one part and then to use the split tool to split off the various parts. The parts would then be brought into an assembly where each part can be worked on individually whilst keeping the other parts visible in ghost mode.

Is this a good way to go about it or are there better methods?

that’s a pretty good workflow. Especially with organic forms. You’ll find that with 10 people, you’ll hear 11 ways to to do it.

When I’m feeling really lazy or in a rush, or just doing for rendering, I’ll work on everything in 1 part file by keeping the different “parts” as separate bodies. SW lets you have multiple bodies in a single part file. At the end, everything can still be broken out as different part files, then re-organized as a proper assembly.

Well, I’m going to sound like a boring teacher, but to start off trying to run before you can walk is never a good idea. :smiley:

I’m going to give you a tip, but first I think you might be missing a vital piece of workflow information regarding Solidworks:

The “convert entities” tool. This essentially lets you go into any sketch of any feature and “borrow” it for your new sketch.

With this, you never need to “match up” your different parts, because they will always be positioned “in place” (when you make a new part, and Solidworks asks you where to position it, just click the front plane of the assembly, and then cancel the current sketch and create a new one wherever you like, even on a plane from another part).

But ok, now for the tip, but remember, this is a quick and slightly dirty way:

Model everything in one file, one part. But don’t cut anything. Just deselect the “merge” option whenever it appears and you feel it is appropriate (double check by hiding your different solid/surface bodies in the feature tree). Then at the end, simply take turns deleting all but one body for export.

Done! :slight_smile:

EDIT: Ha! Beaten while typing my answer. This forum sure yields fast answers some times!

:slight_smile:

Instead of deleting and exporting, just go to the “Solid Bodies” folder and right click on any body, and select “Insert into new Part” This creates a new part that is linked to the original body in the original part. It maintains history too, until you break it.

Get comfortable with the “Feature Scope” options at the very bottom of all the feature option windows. It will let you individually select which bodies you want to merge your new feature with. Very, very handy. The default is to merge everything…

Wow, I learned something as well today. Nice!

Some really good info here, thanks. I’ll play about with it.

Another way to model, is to start with an assembly file and then create one (or a few) parts in that assembly with just sketches. You don’t even need the part files these days and can use the “Layout” feature which dumps a 3DSketch straight in your assembly.

The idea is to use those sketches as a framework, to which you will model your 3d parts off of.

It can get complicated, hell even I don’t really know the entire whats-what on it, if you search the Solidworks forums for “top down assembly” you should get some hits.

Layout is completely frustrating in my opinion. I generally start with a central component, then insert new parts into the assembly. Utilizing convert entities, etc. it gets where I need to go. But, there are at least 15 ways to do 1 thing in SW. And none of them are usually very simple.

Playdo- your method is a decent one. The answer is somewhat dependent on how complex your design is and how powerful your computer. Convert entities, copy surfaces etc also known as in-context modeling can start to slow down the model if there are too many external relationships, especially something beyond simple copying contours.Master modeling/Top down modelling is much more intuitive for designers, because you get a feeling for the gestalt of the shape/function. However it too has issues. The more you have built into the one master model, the longer your rebuild times. If the parts have no tangent surface relationships and are somewhat blocky; maybe sourced /bolted components, then you dont have to worry about a master model and you can create assemblies from the bottom up.

My workflow for master-models is to create the basic volume, without details and then split them up with cutting surfaces. Both the split command and the insert part method will work but can be very finnicky. You have to almost be certain that you are not going to be adding or subtracting volumes after the split. This is because Solidworks can be confused if certain bodies disappear or new ones are created. You have to be relatively certain of the design before the split. My personal rule of thumb is to start splitting once the rebuild times start to be uncomfortable, then insert bodies into new parts to continue detailing. Ideally as soon as the basic form is realized, then start splitting, but I have been burned a few times so I tend to hold off splitting as long as possible. I have had the initial import of the body fail a few times because of core changes in the master model.

I’ve been looking at Convert Entities. From what I gather, Convert Entities can only be performed by selecting a plane and going into sketch mode, then pressing the S key and selecting the edge or surface to convert. The converted edge/surface will then be duplicated onto the sketch plane.

How do I convert an edge/surface and keep the duplicate exactly where the original is in 3d space? eg. for times when the original edge/surface is not on a flat plane but for when it’s curved. (I’ve attached an example image, where I’d like to duplicate the surface in pink as the base of the next shape/part).
Spout.jpg

I believe you have to be in 3D sketch mode for that. 2D sketch must be on a flat plane.

Offset the surface with a distance of zero. :wink:

Just be careful of abusing “proper” SW workflow too much. :slight_smile:

I may be missing the obvious here but if I select a plane, then Sketch, then Convert Entities/Offset Entities it will project the edge onto a flat plane and the ‘curve’ will be lost.

And …If I select 3d sketch then Offset Entities is not available.

Ok, say that I wanted a slight offset:
Just referring to the body cutaway and the pink section of the spout: How do I select the pink surface, produce a copy of it, slightly inset it (scale x+y), use this new body as the start of the spout part? Or is my method of modeling incorrect?

offset the surface x mm - use as a reference. The flex command can be used to visually stretch and squash a body. What does the design look like? we can give you better info when we see what you are trying to accomplish

It’s not a design as such. I’m trying to learn how to model in general.

offset the surface x mm

This is what I’m asking, how to offset the existing curved surface to be used as the starting surface of the next part.

What version of SW are you using? You can find Offset Surface under the Surfacing Tab.

Ah, problem solved. I watched a tutorial showing it being accessed by Sketch - S key - Offset Entities, which has caused me problems. Thanks.

How do I do the same for an edge?

SW2010

Insert>Surface>Offset
for surface offsets

Insert>Surface>Extend to move an edge out.

Face curves are an option too.

There are many commands- unfortunately no 3d Curve offset- so it might be worth it to show us a sketch of what you wish to model. Something specific might help.

http://www.productdesignforums.com/index.php?showforum=60 has a bunch of great links for Solidworks models and tutorials. It will get you started.

Thanks for the info. I’ll get something drawn up.