So you have your hard-earned $2,500 in hand, and are ready to invest it in a powerful new machine. After all, that will solve all your performance frustrations inside SOLIDWORKS, right? Not so fast. ‘If I could save you that money, that would be great, wouldn’t it? ‘You just need to understand that how YOU model in SOLIDWORKS is part of the equation, too.’
A critical area to review first is YOUR specific modeling techniques. ‘More often than not, when we investigate ‘poor’ PC or SOLIDWORKS performance issues from our customers, their modeling technique is part of the problem. Unfortunately, it is impossible to build a PC to compensate for poor SOLIDWORKS assembly and modeling techniques. The truth is, PC loads starts to grow exponentially as ‘processing expensive’ modeling techniques add up. ‘If you want to have success with anything, you must first have a plan. ‘We want to avoid PC ‘load expensive’ modeling because we plan to use these parts in large assemblies and drawings. ‘These are the most common missteps we see with respect to poor performance, so let’s ensure you aren’t making these before spending money on a new PC that may not help solve your problem.
Today, we’ll talk about Part, Assemblies, and Drawing techniques, and examine some of the best practices that will allow you to be more productive, while sacrificing as little as possible. Our goal is to reduce the time you spend sitting around and waiting for a model to rebuild, and instead get you back to designing sooner.
Swept threads on fasteners, pipes, or fittings:Nothing will kill your performance faster than using swept or swept cut threads (commonly found in McMaster-Carr downloaded parts) throughout your assemblies. ‘Please try to use the SW Toolbox components with the cosmetic threads instead. ‘Even the ‘schematic’ configurations on SW Toolbox parts with the revolved threads add up to tax your system because hardware is used so many places inside assemblies. ‘If you have to use parts that include these swept features, modify the part to delete them from the feature tree. ‘McMaster is a fantastic place to get SOLIDWORKS files, just please delete/suppress the thread features in them first. ‘Here is where a small part modeling misstep is multiplied to become a huge PC crushing mistake in your assemblies. ‘How many fasteners are in your assemblies with swept threads? ’50, 100, 200? ‘Your answer should be 0. ‘Hardware threads should be represented by simple, cylindrical geometry if you want to minimize your PC load.
Unnecessary detail modeled on parts:We get it. ‘You are very detailed oriented and must model down to the last patent number, logo, recycle code, warning label, painted over gnat, and/or swept wire in your parts. ‘While those are great traits for an engineer to have, do you really need those features in your parts, drawings, and assemblies? ‘You can save a lot of time by not modeling those in the first place. If you must have those details, make a reduced detail configuration where those features are suppressed. ‘We don’t want you to be lazy, we want you to model efficiently. ‘Use ‘feature statistics,’ on the evaluate tab the command manager to help identify your heavy load features. ‘Below are some of the top offenders:
- Extruded/Embossed/Debossed text: Use a split line feature if you must have text on parts. ‘It’s much less taxing on the video card because it doesn’t create the hundreds of small depth surfaces from the extrusion. ‘You can also use a decal if you have an image of your text/logo.
- Transparency: Please turn this off if you can. It significantly adds to the geometry detail your machine must draw. Having transparent parts can increase the load on your GPU by up to 40%. We recommend only using this for renderings in large assemblies, otherwise hide those parts or make them opaque.
- Large pattern features: Please try to suppress these in a special low detail ‘for assembly’ configuration. Patterns are better than separate individual features, but can still multiply a load on your PC.
- Fillets:’These start to add up on commonly used parts. Avoid/suppress them if you can on ‘high BOM quantity’ parts in your assemblies. Ask yourself if you really need .010in fillets on all edges to finish this design? Create a configuration where you suppress them for use in assemblies.
- Imported parts:Ensure your imported parts are solids and have a sane number (generally <10) of bodies. Surface bodies add up quickly and are often much more taxing than a single solid, due to the nature of surface definition. There are options to try to create solids when importing parts in SOLIDWORKS, make sure you have these checked. Try to merge multi-body parts into a single body. These imported parts can use up valuable GDI objects if they have a large number of bodies inside them. Windows only allows 10000 GDI objects as an OS. This is a fixed, finite OS resource that can easily be max out. SOLIDWORKS (or any other Windows program) crashes to desktop when it goes over this limit.
Mates:SOLIDWORKS is great in that it allows you the freedom to mate to just about anything. Should you always follow this kind of careless behavior? Probably not. This is an area that starts to add up when your assemblies grow in size. You should always follow a plan:
- Mate to primary planes or axis:This is such a critical ‘best practice’ for so many reasons. You will never have mate errors again if you can do this for every part. Of course, we realistically cannot mate EVERYTHING to a default plane, but do the best you can. It also reduces solve time in assemblies because SW doesn’t have to resolve the part geometry before solving the mate. The primary planes are always there, so build your large assemblies referencing items you CAN’T DELETE and use them in mates. You wouldn’t build a skyscraper on a sandy foundation, so don’t do the equivalent with your large assemblies.
- Mate to part level planes or axis: These items are more robust than part faces, and are less likely to cause errors. In fact, when they do error, they are easy to fix in the part environment. If you simply mated to part faces in an assembly, you must trouble shoot the mates in a much more complex assembly environment and may not find the problem until years later when you open the assembly and it is updated.
- Always mate components to the assembly level primary planes/origin:You don’t want to have your parts floating relative to the assembly origin. This creates another unknown for your PC to solve. Lock components down to the assembly origin. It’s a good idea to minimize the degrees of freedom (DOF) for as many parts as possible. Do you like doing math problems with 100s of unknown variables? No? Neither does your PC.
- Mate logically; avoid sequentially: This is another instance of ‘just because you can, doesn’t mean you should.’ Mate remove degrees of freedom. When you ‘stack’ together mates, you stack together equations that SOLIDWORKS must solve. When you have several components mated to a common part, mate them that way, rather than tying them together.
- Use assembly patterns/mirror: This greatly reduces the individual mates in your assemblies. It also saves you time if something goes wrong because you just have to fix it in one place. The pattern feature does the hard work from there. Don’t ‘drag and drop’ each fastener into your assemblies. Drag one, then use feature driven patterns and assembly mirrors to populate the hole-wizard hole series. If you aren’t doing this already, you are doing it the hard way, for both yourself and the PC!
- Use sub-assemblies:A good rule of thumb is not to have more than 1 screen’s worth of parts/sub-assemblies inside a single assembly. If your assembly feature tree has a vertical scroll bar, it is probably time to start creating more subassemblies. If you have repeated part patterns, create a sub-assemblies and pattern them.
- Excessive DOF in linkage based assemblies:Try to avoid having complex mechanisms that are able to exercise inside Solidworks. This involves a lot of complex math to resolve the final location and may also have multiple solutions depending on your mates/components. You can suppress these mates to free your mechanism during design, but try to keep it fixed after you test the range of motion.
Assembly level features:These are generally very powerful techniques and can save you time modeling. Just make sure they don’t end up costing you time on the backend when you get to your top level assembly.
- Avoid creating assembly level planes or sketches that are a result of other mated components:Your PC must first resolve all part geometry, the location of those parts and mates, before it can determine the location of the plane or sketch. This becomes taxing if you then mate other components to that assembly level plane. This is a long mate solve tree for your PC to solve.
- Avoid using flexible sub-assemblies if possible: This is a great feature inside SolidWorks, but it doesn’t mean it should be used without discretion. It can be very taxing on your PC. It is usually better to model movable components in the top level assembly where they move instead of using flexible sub-assemblies.
Finally, a Note on Drawings
SOLIDWORKS is great in that it has relatively few rules when it comes to drawings, but that doesn’t necessarily mean you should have your own. Try to avoid putting multiple parts/assemblies in the same drawing file as these start to multiply PC load quickly. Also try to minimize the number of sheets inside a drawing. Your PC must simultaneously open all referenced parts/assemblies once they are shown in a drawing view. Create separate drawing files to cut the workload on your PC down to manageable levels. Alternately, use the ‘Select Sheets to Open’ option, from the open dialogue to lighten the load for a single drawing.
If you think about performance before while you are creating the model, you’ll really squeeze a lot more productivity out of even a less powerful computer. You’ve just got to be willing to recognize that even though your computer may be the bottleneck, there are things you can do to help.
I hope you found these tips and best practices helpful. I apologize in advance if this deprives you of taking your coffee break while the model rebuilds! All in all, our goal is to help you get more done.Thanks again for reading.
If you’ve read this, and still need some hardware recommendations, please see Building a Cost Effective Workstation for SOLIDWORKS 2016.