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When I field questions or issues from SolidWorks users about some trouble they are having modeling in large assemblies or very large assemblies, two main aspects come to mind. First is this a Hardware/Operating System limitation? Second is this a Modeling/Organization performance issue? To answer these questions in depth would be quite a long read, so in this case I will keep this to its simplest terms.
Hardware / Operating System
How much system RAM do you have installed 1GB, 2GB, 4GB?
If you are using a 32bit version of Windows XP or Vista you will be limited to 2GB of RAM unless you have the 3GB mode enabled in your boot.ini file.
Even with this mode enabled and 4GB of RAM installed you will still be limited to somewhere between 2.5GB - 3.1GB useable for SolidWorks and other software, depending on how your system BIOS is programmed to use this memory for your installed hardware and operating system. Large assemblies can run right up to this RAM limit and cause yours system to Slow or even crash.
If you find you are running into this limit in your large assembly modeling, there are two solutions.
One option is to move to a new hardware system that uses a 64Bit operating system like Windows XP 64Bit Edition, install 8GB of RAM or more and get the fastest processor you can afford. The 64bit operating system and compatible hardware offer a much higher limit of available RAM, the current hardware limitation is about 64GB. The other option is to use modeling techniques that cause less data to be loaded into RAM and less data to be processed by your CPU allowing the system to run faster and make working with large assemblies in SolidWorks more enjoyable. Which brings me to the second part of this article.
Modeling / Performance
SolidWorks has two modes that help with large assemblies they are “Large Assembly Mode” and “Lightweight Mode”.
“Large Assembly Mode is a collection of system settings that improves the performance of assemblies”
This mode can be toggled on from the tools menu. Below is a list of options effected by this mode setting.
System Options page or Toolbar |
Option |
Status when
Large Assembly Mode is on |
Drawings |
Show contents while dragging drawing view |
Off. Only the view boundary is shown while dragging a drawing view. |
Smooth dynamic motion of drawing views |
Off. Dynamic operations to drawings, such as panning and zooming, do not display smoothly. |
Automatically hide components on view creation |
On. Any components of an assembly not visible in a new drawing view are hidden and listed on the Hide/Show Components tab of the Drawing View Properties dialog box. |
Drawings - Display Style |
Display style for new views |
Hidden lines removed is set as the default display style for new views. |
Display quality for new views |
Draft quality. Only minimum model information is loaded into memory. Some edges may appear to be missing, and print quality may be slightly degraded. |
Display/Selection |
Dynamic highlight from graphics view |
Off. Model faces, edges, and vertices are not highlighted when you move the pointer over a sketch, model, or drawing. |
Anti-alias edges |
Off. Jagged edges in Shaded With Edges, Wireframe, Hidden Lines Removed, and Hidden Lines Visible modes are not smoothed out. |
FeatureManager |
Dynamic highlight |
Off. The geometry in the graphics area (edges, faces, planes, axes, and so on) is not highlighted when the pointer passes over the item in the FeatureManager design tree. |
Performance |
Transparency |
High quality for normal view mode. While the part or assembly is not moving or rotating, the transparency is high quality. When moved or rotated with the pan or rotate tools, the application switches to low-quality transparency, enabling you to rotate the model faster. |
Curvature generation |
Only on demand. Initial curvature display is slower, but uses less memory. |
Level of detail |
Minimum. The level of detail is minimal during dynamic view operations (zoom, pan, and rotate) in assemblies, multi-body parts, and draft views in drawings. |
Check out-of-date lightweight components |
Don't Check. Loads assemblies without checking for out-of-date lightweight components. |
Update mass properties while saving document |
Off. Does not recalculate the mass properties on save. The next time you access the mass properties, the system will need to recalculate them. |
View toolbar and menu |
Shadows in Shaded Mode |
Off. |
RealView Graphics |
Off. |
The Lightweight Mode, when a component is Lightweight, only a subset of its model data is loaded in Memory. The remaining model data is loaded on an as-needed basis.
You can open a model lightweight by going to file open, selecting the model, and then make sure the lightweight check box is checked before hitting the open button, Or under tools, options, in the performance menu select, assemblies, select Automatically load components Lightweight.
Beyond using the “Modes” to help with performance the biggest benefit is going to come from proactive modeling. Recognizing that the parts, assemblies and subassemblies you are creating are loading a lot of data into the system and building them to be efficient for this reason.
Below is a list of techniques for minimizing data load.
First Rarely if ever do you need to work or build your assembly in a fully resolved, default configuration. Avoid it at all costs.
Second build all your Parts with a simplified or assembly configuration that has a minimized number of features unsuppressed to represent the part. Suppress things like fillet, chamfers, small or internal features that are not going to be functional in the assembly. Use your “feature statistics” from the tools menu to help you determine what features use up the most resources and see if you can suppress them.
Third build simplified configurations of your subassemblies with the simplified parts in them.
Fourth build simplified main assemblies with the simplified subassemblies in them.
Fifth build “No Hardware” configurations of your main and subassemblies that have fasteners and other hardware suppressed.
Sixth try to limit the number of top-level mates in your main assemblies build these into your sub assemblies. You can see where you are at with your “assembly statistics” from the tools menu of your assembly It is better to have more subassemblies.
Seventh try to build your assemblies to a bill of materials that may already be laid out in planning it will help with the organization of subassemblies.
Last building these assemblies with simplified parts will also make drawing documentation perform much better, the opening and rebuild times of drawings will be dramatically improved.
This focus on Hardware/OS options and Proactive assembly modeling techniques and will reduce frustration with performance issues and improve your product time to market.
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