Quick Solidworks Question - create separate part from an existing part?

[fuzzybabybunny]

I created a part file and I basically created two distinct parts in that part file:

http://paragon.media.storage.s3.amazonaws.com/Solidworks Part.JPG

I want the thing in blue to be made into its own separate part. How do I do that?

The reason I made two distinct parts within the same part file is because the measurements from part 1 are needed to make part 2, and it is WAY easier to make the second part when both parts on in the same workspace as each other.

I'm a complete noob at SW so I'm not sure how to create two distinct parts in separate part files and still be able to easily see / reference the measurements of the first part to create the second part.

 

[effowe]

You have two components in one file. You need to separate those into their own components and then create an assembly that references them.

http://help.solidworks.com/2012/English/SolidWorks/sldworks/Assemblies.htm

 

[RGUN]

Just use configurations to show one at a time. Note that this is a workaround and top down design would have been the better solution.

 

[edro]

The quick and dirty way would be to do Save As so you have 2 part files that are identical.
Open one part file, create a protrusion/cut/extrude (whatever SW calls it) that cuts away the entire blue part.
Open the other part file and do the same thing to the gray part.

Create a new assembly file and insert the first part using the part datum planes with align constraints.
Add the second part to the assembly using an axial constraint on the hinge, and some align offset constraints to line it up.

BTW, you can create parts while in the assembly environment. All 3d cad packages allow this.

 

[yottabit]

You can "delete body" for the part you don't want and then save a copy as someone mentioned

I prefer to do it by inserting the original part into a new part document to create my mating part, and then at the end split and delete the inserted original part body. What this does is keep dependency to the original part you are modeling off of. By inserting the original part into your new part you would only see something like "originalPart" instead of all those original part cut/extrudes, and it would be linked to the original file.

One plus side to this approach is if you make some changes to the original part and the stars are in alignment (aka it was dimensioned sensibly and with some foresight) your mating part will automatically update.

The best thing to this approach in the real world though is that it removes any fear that you may have your mating part working off the wrong version of the original part. For instance I create OrigPart1 and MatingPart1, then OrigPart2 and MatingPart2. Revisiting the files months later, you may ask yourself "wait a second, is MatingPart2 actually based off OrigPart2 or is it based off OrigPart1?" If the files are linked you will instantly see the file name the mating part was modeled off of- if not you'll have to try to tell by the feature tree (which can be not fun if the types of changes you made were ~.001"!)

Edit: Also if you are new to Solidworks the best advice I can give is to make your own set of sensible keybinds, it will save so much time. The biggest ones for me are I bind D to Smart Dimension, Shift+M for Assembly Mate.

 

[fuzzybabybunny]

Thanks for all the tips guys.

I'm having some issues with this whole workflow thing.

It seems to me that in order for this to be as intuitive as possible, it should be top down and mimicking an actual workbench.

As in, start with a blank canvas. This is where the final assembly is going to be.

You start by making a part in the assembly canvas.

Then you make another part on the same canvas right next to the first part you made, creating references and links between the parts so that they can change with each other. The idea is to make and modify the parts in the exact same workspace so that they can easily reference each other, or reference the central part, like an engine block.

Then you simply highlight an entire part, name that Part 1, highlight the second part, name that Part 2, and in that way you will be able to create the individual part files and open them up separately as just part files if you ever need to.

Right now I have an Assembly open. I select a plane, make a sketch, but there are now no options to extrude. In the assembly canvas there should be an option to not just INSERT a component but also to MAKE a new component, no?

 

[Danadcorps]

No. Assemblies are to put together part files. What you should be doing is creating the individual parts. Then use the assembly to put all the parts in and create the mates.

Btw, when you create parts, use the natural planes to help with your mates. Center your work and use plane references where needed. That way, when you want to create mates, you can do so using a natural symmetrical plane instead of "assuming" that you made it symmetrically. A guy at work never creates his parts like this and it irks me when creating assemblies 'cause now I have to find the dimensions and halve them instead of just using planes (then again, when using someone else's work...you should always measure to make sure).

 

[EEK22422]

Right now I have an Assembly open. I select a plane, make a sketch, but there are now no options to extrude. In the assembly canvas there should be an option to not just INSERT a component but also to MAKE a new component, no?

You are actually correct. If you go under the Assembly ribbon, click the arrow "Insert Components" and there is a "New Part" option. From there go to your sketch ribbon and select a surface to work off of.

Making entirely separate parts and putting them into an assembly is a basic use for SolidWorks and not the most efficient route for complicated, interacting designs.

You can easily make a part file, which contains multiple bodies into an assembly without having to manually create any mates. This is a great resource I used to learn this skill: http://gupta9665.wordpress.com/2010/11/10/assembly-from-part-no-mates-required/

Hope this helps!

 

[sm625]

It seems to me that in order for this to be as intuitive as possible, it should be top down and mimicking an actual workbench.

You need to give up on the whole notion of intuition when dealing with solidworks. The program is garbage. I had to create a 3D print job a couple times and it was a nightmare to use that software. But you can eventually muddle through it. I wouldnt worry too much about it if you end up with your own unique way of doing things. Creating multiple parts you want and them breaking them up into chunks and saving each piece might be the best way to do it. That's probably how I would do it. I guess it depends on how much you're going to be using the software. For me its just a couple little projects a year and so I do not want to have to waste 2 days fiddling with a POS tool to do a design that should only take a couple hours.

I remember trying to do the tapering on 4 cutouts. They were similar but for every single one I had to take radically different steps because the software is so buggy that nothing worked repeatedly or consistently. On the last one I got completely stuck because it simply refused to work. I just basically ended up starting over because it just wouldnt do what I wanted, even though I was on the 4th frickin one had done it 3 frickin times already and it was the same operation.