Making Drawing From Print

This humbled newby is back. So far I'm 1 for 1. Here it is:

I created a shelf as one whole part. I used to make each part of the whole and save them to create an assembly. That would allow me to take each part and make a drawing out of it. I found it quicker to make the whole finished product as one part. But, now I want to make a drawing out of each individual section of the part, for example the rear aluminum strip that mounts to the wall. Is it possible to make a drawing of each individual part of the whole part when it is created as a whole? I've tried to copy an extrude from the whole part, then paste it on a new "part" ( to make a drawing out of it). But then I realized that it was created by making a sketch on one of the sections of the part and wouldn't work because it's reliant on it. I've dragged the tree to the top so that only the first part of the whole was showing (Rear Mount), but then I realized that I wouldn't be able to do that to anymore of the whole because as I dragged to the bottom, everything would be shown. I would have to delete the previous parts of the whole. So then I thought that maybe I would create an assembly, then separate the whole thing. But I don't know if the dimensions would show. I hope this makes sense. It's rather confusing. Any help would be much appreciated. Thanks in advance.

I think this thread should be in the 3D section - may get more help there...Any Mods that can help out here?

Are you talking about Inventor multibody parts? If so you might be better of useing thr 'Make components' tool in the 'Manage' tab to create an assembly from your 'Master' part. This will give you the fexibility you are looking for.

Well I want to make a drawing of all of the individual parts that make up the whole part. I don't want to make each part separately then assemble because it takes longer. When I do it that way, I can just open each individual one then make a drawing of them. When it's all one part, I can't seem to find a way to separate them. I'll try on the 3-D forum.

I'll check the make components tool and get back to you. Thanks a lot.

We're talking Inventor or AutoCAD here? It's your use of the word "assembly" that makes me ask.

I'm sorry. I should have been more specific. It's Solidworks 2008 Auto Cad.

So this is an Inventor question? Not an Autocad question?

There's no such thing as Solidworks 2008 Autocad. Are you using Autocad or are you using Solidworks?

Ooops Sorry, Solidworks 2008.

I have merged your two threads and moved them to the Solidworks section. In the future, it would be best to post your questions in the appropriate area of the forum in order to get advice that's relevant to your software.

Paul. You can create a new part from your multibody part. At the top of your feature tree there is a folder called SolidBodies. If you right click on any of the solid bodies there will be a "make part" option in the menu. This will create a new sldprt file. You can also make use of configurations. You can create multiple configurations where each configuration only has one of the solid bodies. You can add features(such as Delete-Body), you can hide or suppress things like features or entire parts. The method will really depend on what the end result you are looking for.

If I understood the question correctly you have a part with multiple bodies and would like to make a drawing of each body. If this is the case you can accomplish this by adding a relative view in your drawing file. Just start a new drawing, insert any view, right click on view and select drawing view then relative view. This feature will direct you to the part file. You will have the option to select specific body's and how to view them. Is this what your trying to do?

Ooops Sorry, Solidworks 2008.

When you made the individual features in SWx you had the option of merging features as one solid or modeling as multi-body solids. You should have unchecked the merge feature tickbox as appropriate.

Given the difficulty figuring out what program you were even using for this problem, perhaps it would be a good idea to zip and attach the file here for further instruction.

The program is Solidworks 2008. I did uncheck the boxes so that it didn't merge all of the body's together. So that's not a problem. But I think the solution is above. I'm going to have to try it out when I get home today. Thanks though :-)

Thanks guys. I'm going to see what I come up with when I get home tonight. I appreciate the help. I'll let you know if I figure it out tomorrow.

shift1313 & bhamze. Both ways will do it. I knew I picked the right website. Thanks again :-)