Assembly drawing super slow, please help.

You call that slow? You ain't seen nuthin. You can't even take a powder and get a cup of coffee in that time.

Bet you want some practical advice too. This is what helped me:

1. Remove all fasteners from the assembly unless absolutely needed.
2. Have configurations for parts with fine detail removed.
3. Make sure that all mates are robust and cherry free.
4. Hide all complex views you aren't working on at the time
5. Work in shaded mode and draft mode till you absolutely must have it the other way.

What video card are you using? Going from a std consumer type card to a fire gl T-2 was the best $200 we ever spent on hardware. Even if you have a good card, its worth trying different drivers, if even only to eliminate them as a cause.

Monitor task manager. Check your memory useage. If "Commit charge total">("physical memory total"-"physical memory available") by more that

Turn off the system-drawing options for smooth dynamic motion and show box contents while dragging, unless you have to have them at the time. Ensure that your document properties image quality has not been messed with (ie. you turned it all the way up so that you could select a vertex that was being a PITA, but forgot to return it to a reasonable value).

If any of your drawing views are shaded, check to see if any of the visual properties have been altered. Optical properties other than default are resource hogs. Check to see that no materials or textures have been added unless required. I think someone has a macro that resets all visual properties and assigns random colors to each components that might be useful here.

I can't fully understand this one, but, fonts other than standard windows/sw ones seem to cause me lots of problems even when TT.

Create a new configuration for your assembly and place a fresh view of it on a new sheet. Supress components in groups to see if its an issue with a single sub-assembly or component. I have an actuall full model of 2 1/2" diameter 10" length perforated tubing, 3/16" holes on 3/8" centers, staggered pattern made from sheet metal. It will bring any system to its knees.

Not better? Try unsupressing all components and supressing all mates (provided you do not need dynamic motion or require further updating). Fix all components.

Good luck!

Thanks TOP and Brian for some nice tips. We already do a bunch of them, but some are new to me.

One thing I wish they had is a "2D" mode. Even though drawings are 2D, SolidWorks still has the 3D model loaded in the background. This mode would let you work in 2D, and if the model is changed, you then have to update your views. This might not be possible with SolidWorks, but it would speed up drawings greatly.

The question you have to ask about this is how do you get the 2D data? It has to be generated from and driven by the 3D data. Especially things like intersections of curved surfaces simply don't have a 2D meaning.

Correct. But after it grabs the information from the 3D model, then convert it to 2D so you can work with it must faster. If the model is changed, then the drawing will update the data.

What bugs me is when I do a simple detailed view. Sometimes edrawing viewer see the entire model at the scale of the detail view, instead of the windows detail you want displayed. Now im getting into viewer problems, but if the drawing was simpley a 2D lines, then you wouldnt have that problem.

Just a thought, maybe its very complicated to do...

I haven't tried this at all, but what about using Detached drawings? The whole idea there is to work on the drawing without the overhead of loading the model.

WT

Sounds like detached model would your solution. It has worked very well for me. See the posts on "detached model" elsewhere in this group.

Regards,

Dennis