Matt Lombard’s Five Favorite Tips and Tricks
Here are my five top SOLIDWORKS tips and tricks:
- How to handle top-down design
- Feature Manager management
- Interface setup and use
- Surfacing work
- Manual file management
1. How to Handle Top-Down Design
Top-down design is one of those things that salesmen are quick to promote but technical people are quick to mock because in the wrong hands it can cause some major heartaches and loss of data. There are several ways of handling top-down design, but only two real concepts.
One concept—the typical in-context method—is to make references between parts within the assembly. This can include making references to layout sketches that have fewer layers of problems but still the same underlying issues. This approach works, but it adds a lot of overhead to the assembly, and you have to have the assembly open to update the parts. It is fraught with problems such as slow speed and references getting lost due to file management issues. You also have all of those icons in the Feature Manager.
Companies often require users to delete all references or round-trip export the data at the end of a project. It is silly and unnecessary, but I get it. They don’t understand what’s going on or don’t trust their employees or systems.
The second method is the master model. In the master model, you model the parts that require external references in the assembly as a single part. It could be a multibody part or a single solid, and can be a mix of solids and surfaces. In this way, all of the references for changes and updates stay within the same file.
To make parts from the multiple bodies, use the four master model push or pull type features: Save Bodies, Split, Insert Into New Part and Insert Part. Refer to Surfacing Episodes for a detailed explanation of how these features are different from one another and how to pick which one to use in different situations.
Once you break the individual parts out to separate files, you can put them back together again in an assembly. They will all share the same origin, so they are easy to assemble. You can also add additional features to the broken-out parts. Details, plastic features, shell, draft, mating features and anything else you need can be added after the part is broken out from the master model.
The advantage of the master model is that it does not require an assembly file to control anything. It also allows you to break up the rebuild times for parts that have large feature trees. This means that, for all the detail work, you won’t have all of the initial features rebuilding. This technique requires the master model and the child parts created from the master. You still have to understand and follow some basic file management rules but should you break something, it is easy to fix.
The main disadvantage of the master model method is that you have a master model part file that is not part of the assembly. It won’t show up on a BOM, but you have to have it if you want to make changes.
2. Feature Manager Management
There are two kinds of users as far as I’m concerned: those who make complex assemblies of simple parts and those who make small assemblies of complex parts. I’m typically the second kind. Either way, you can get a Feature Manager full of stuff that needs some special tools and techniques to manage.
There is a detailed article that talks about this topic here.
For Feature Manager management, itis mostly about the tools and how you use them.
- Naming features.
- Grouping features and bodies into folders.
- Using color to identify special faces or features (using the Display Pane).
- Using Freeze Bar to prevent rebuilds.
- Dynamic reference visualization.
- Use the FeatureManager filter.
- Flat tree view shows things in order of creation instead of consuming parent features.
- Gain additional display real estate by detaching the FM or using the flyout FM.
- Navigate with arrow keys.
- Use Scroll Selected Item into View in the RMB menu.
- Split the Feature Manager to see the top and bottom at the same time.
- Hide/Show Feature Manager with the F9 key.
- History folder for parts in assembly shows the features you have recently touched.
3. Interface Setup and Use
Users have different goals for the interface and there are many factors that push your use in a certain direction. Hardware is one factor that influences your interface decisions. Do you have multiple monitors? Is your main computer a laptop? Do you have a 3D mouse device?
Some people may select how they use the interface based on what’s new or what they feel is being sold as “cool” by someone they look up to or trust, and may even assign labels like “old fashioned” to some interface elements. This is an emotional approach. It is true that certain parts of the interface can be inefficient. But there are always ways you can do better.
I judge an interface setup by six criteria:
- Clicks (mouse or keyboard)
- Mouse travel
- Device change (moving hands from mouse to keyboard)
- Setup time/effort
For example, using hot keys is fast but it requires setup, memorization and moving your hands from mouse or 3D mouse to keyboard. Using the radial or RMB (right mouse button) menus minimizes mouse travel but requires setup and two clicks per command. Using the regular menus requires no setup but a lot of memorization, mouse travel and, in some cases, a lot of clicks.
But isn’t everything you do some sort of compromise? Do you use the software all day every day or just once a week? Do you usually repeat an action or feature again and again or is every new feature a chess move?
I personally use the context menus—the right and left mouse button clicks that bring up contextually sensitive menus usually have the things you’re looking for when a specific item is selected.
If I’m doing a lot of specialized work, I might set up hot keys. Hot keys work best for stuff you do frequently and can remember easily. If you have to look it up on a list, it’s not helping.
4. Surfacing Work
Not everybody uses surfaces. Some people who don’t really should and some who do really shouldn’t. You should only use surfaces in these specific situations.
- You cannot make the shape you need using solids (organic shapes).
- Using solids would be inefficient (splitting a mold),
- You have to fix a badly translated model.
- You have imported a surface model for reference.
If you need to do this, take some time to look at some examples. Get comfortable with managing bodies in folders, using color (for identification) and all of the body manipulation tools you need to trim, knit, intersect, split and otherwise manage surface bodies.
Solid modeling actively tries to make a single solid body for you. Surface modeling, by default, makes a new body every time you make a new surface feature, even if it touches other surface features. It’s a different way of working.
Also, be aware that history-based CAD is not necessarily the best tool to do organic shapes. Consider tools that include T-splines, sub-D modeling or other push-and-pull type shape manipulation.
5. Manual File Management
When starting out with a new program, you are left on your own to manage the files. Some people take the folder approach; others put all the files in one big folder. Some try to get fancy with revisions or projects, or the function of the part.
SOLIDWORKS uses a system of searching for references and if you make changes or create copies, you will probably break a bunch of the references. In the beginning, we all make mistakes and sometimes make bad mistakes.
Manual file management can depend greatly on your part numbering system. There is a lot to say on this topic, but in the end, my bottom-line recommendation is to use a system with a semi-intelligent part name that allows you to identify the type of document quickly by sight, but which has in it a sequential number. Some special part types might have an identification suffix, which is also smart.
The irony is that manual file management is thrust on beginners but requires the knowledge of a veteran user. Only users with a lot of experience and knowledge can set up a manual file management system that will always work.
However, anyone with that much experience and knowledge knows that manual file management is one of the most dangerous things you can do with your company’s data.
The simple solution to manual file management is not to use it. Get an automated file management system like DBWorks or one of the SOLIDWORKS PDM applications. Unfortunately, any automated file management system will require a lot of specialized knowledge, training and maybe different skills.
An automated file management program enforces all of the best practice rules for file management. People get in trouble with file management by not knowing, not understanding or simply not following the rules. Sometimes the tools meant for manual file management are limited and not understanding those limitations can also cause you problems. For example, a search might only search where you tell it to look, it may not be able to find parts that have been moved off the network or to a folder out of your search area.
If you still feel like you need to use manual file management, here are some rules you have to follow:
- Use unique file names—always. The extension counts as part of the name.
- Do not put revision level in file name (unless it is for obsolete revisions only).
- Do not separate parts/assemblies/drawings into different folders—you have to maintain links between documents.
- Don’t use configurations for different part numbers.
- Don’t use configurations for revisions.
- Use Pack and Go, SOLIDWORKS Explorer/SOLIDWORKS File Utilities or SOLIDWORKS itself to copy, rename or move anything that is referenced by other documents or references other documents (such as parts, assemblies and drawings).
- Put shared library files in a centralized shared network location.
- Projects can all be kept together in a folder or sub-folder structure as long as they are put there when created or moved there using the tools mentioned above.
- File names should be part numbers, the description should be a custom property
- Revision should be a custom property.
- Decide which documents are release/revision controlled—drawings for sure, but how about parts and assemblies?
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