Detail part on assembly drawing?

[MechEng2005]

My current employer is transitioning to SW (from 2d) and I was hoping somebody offer some advise, tips, or knowledge.

We use a lot of parts defined within assemblies. Virtual parts works great for this. I can define the part within an assembly and mate it, but it doesn't require it's own part file. However, some pieces may have a number of features. When I get to the drawing, I would like to be able to provide a detail of the part.

I know that if I had an assembly and wanted to make a detail view of an isolated part that was saved externally from the assembly (in its own part file) I could add it to a drawing by browsing to the file. However, this doesn't work with virtual components. Even if I open the virtual part, and then go to the drawing to add a model view, it doesn't recognize the part as being available for making a drawing view.

Is there any way to create a drawing view of a virtual part in a drawing of an assembly? Currently, I have to bring in a drawing view with the component orientated how I want, and then hide all other components in the drawing. Is there a better way?

-- MechEng2005

 

[Updraft]

Maybe such a part should no longer be a virtual part and should be converted to a stand-alone part.

- - -Updraft

 

[gwubs]

I would strongly recommend modeling parts, drawing them, and use assemblies and assembly drawings to detail how the parts go together. This will allow you to get a grip on revisions, to name only one thing. The only information other than pure assembly info (eg. BOM and part location) on an assy. drawing is that for an operation that occurs at assy level ie. drill on assembly & etc.
It IS worth the work to do things this way in my experience.

 

[ShaggyPE]

I don't see much value in the whole "virtual part" methodology... except for sand box conceptualization. At some point it should be broken out into parts and assemblies. IMHO

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[Updraft]

Dustin,

We don't use the VP very often, but as it was first introduced to us it was a convenient way to include items in the BOM that did not need their own drawing. This would include grease, thread locker, paint, adhesives, etc. Some have even advocated using VP for purchased items, such as compression fittings, though we prefer to have those as parts, even if we don't make a drawing of them.

Many ways to skin a cat.

- - -Updraft

 

[rgrayclamps]

Hi, MechEng2005:

You can add a detailed view of a virtual part in your assembly drawing document although I do not enourage you to do so. Below are steps you need to add the view:

1) Open both your assembly drawing and model documents;

2) Open (right click) your virtual part in its own window;

3) Insert a "Relative to Model" view to onto your assembly drawing document;

4) Select orientations of the view from your virtual part.

You will see a "Relative to Model" view of the virtual part added to your assembly drawing document.

Good luck! Have a nice Thanksgiving Holiday!

Alex

 

[mjcole]

Check out Configurations and Display states to achieve this.

Save Bodies might be another way to do this it will insert the Features of a body as an External link in a new Part. You can then Right Click the Link and pick Edit in Context to get to the Master Assembly file and your Features in the Virtual Part.

Have you ever gone to make a Drawing and been told by SolidWorks this model must be saved to create a drawing?

This is because SolidWorks uses linked files to pull data from a part to the Drawing. You can try to find the temp directory that SolidWorks uses to put the virtual parts on disk.

Michael
Happy Day

 

[MechEng2005]

Thanks Alex. That's what I was looking for.

Concerning when to make stand-alone parts, I have used SW with previous employers and we typically did stand-alone parts for each piece (although even then, there were exceptions). Where I'm working now, there is some resistance to change, and many people are still sticking with doing things in 2d since they are familiar with it and it is less frustrating than learning new software. Since I've used SW at previous employers, I've ending up spearheading the transition from 2d to some extent. It will be difficult enough getting everybody to use the software to create drawings that look basically the same as what they are used to. If we start changing "the way things have always been done" I'm afraid there will be push-back from throughout the company and we will let the Solidworks software rot and stick with 2d. I do think we need to change the mentality that the only way to do things is the way they've always been, but slowly, one step at a time.

-- MechEng2005

 

[MechEng2005]

UPDATE:
Alex's method did what I was looking for, but it is bugged. I used Alex's method to create detail views of parts on the assembly drawing. However, everytime I opened the drawing all the views of the virtual parts were missing (dashed lines making a box with an "X" in it were the view should be).

If I RMB, select show, it would give an error message (I forget exactly what it said). Then, I would have to RMB > Properties and change the configuration button from "Last used config" to "Named config" or vice-versa. It did not matter which one it was set at, it just needed to be changed. Then I could RMB > Show and the view would show up along with any dimensions and annotations associated with that view.

I talked to my VAR and he verified the behavior on his setup and submitted a notice to SolidWorks. So even with Alex's method, I still can't use virtual parts and have them detailed on the assembly level. Although, I can do this if I save the part as it's own file (non-virtual part).

<sigh> Nothing can ever be easy...

-- MechEng2005

 

[aferro]

Hi,

i read your post only today, and i don't know if you solved your problem. If not, in our company we used to work with assemblies, and (even if it's not correct) we put the detailed parts in the assembly drawing.

To do that, and with parts existing externally, we NEVER browse looking for the part; but we do:

MODEL VIEW - and we click on the part on the drawing (it's faster).

The problem is with virtual components, and you solve it with

STANDARD 3 VIEW - clicking on the virtual part on the assembly drawing view (and deleting the views you don't need)

Also, "standard 3 view" is a good solution to mantain the right configuration of the part in the drawing, especially if you have the same part in a assembly with two different configurations, and you want to have a detailed view of both (with "model view" the results are not accurate, it often opens the last saved/opened configuration).

Hope it helps,

Alvise