Have you ever struggled with rebuild errors or out-of-control 3D CAD model complexity? This article includes tips and guidelines for how you can plan out your individual part models, as well as project planning tips for tackling assemblies.
Although they are SOLIDWORKS focused, the methodologies discussed here should be relevant to any feature-based CAD software. This article is a companion piece to a presentation given at SOLIDWORKS World 2019, which can be accessed here in both the PowerPoint and recorded presentation featuring live demonstrations of many of the techniques described.
Establishing a Model Plan
I’d like to present a simple workflow (see Figure 1) that, in the absence of a more sophisticated strategy, can serve as a basis for creating a robust CAD model.
As much as possible, features should reference back to the reference geometry and initial sketches that are planned out after a clear outline for the model has been established. The success of this process also hinges on performing checks during the modeling process—correcting and reorganizing as you go to make sure your work remains conformant to the plan.
Figure 2. Making a hand sketch of an outline.
Hand sketching an outline as shown in Figure 2 is a highly recommended prerequisite before you begin the modeling process. This sketch attempts to define the overall shape of your model and a few key parameters that will be driving the model’s design objective. It’s much better to figure this out at this stage rather than after you already have a lengthy feature tree.
To create your sketch, all you need is pen and paper (and, as you can clearly see from Figure 2, you don’t have to be an artist). A quick smartphone picture will digitize the sketch for your records. Unless you are completely confident that you have a clear mental picture of the end result in your head, don’t skip this step!
From the hand sketch, think ahead to what major features will make up your model. This will help guide the structure for sketches and reference geometry that will be created in the next steps.
Create reference geometry and initial sketches (see Figure 3)—these are the planes, axes and sketches that will be used to create the majority of the part features. Creating the appropriate geometry requires “thinking backwards” from the features you are planning to generate. Having more reference geometry than you need is fine, as extraneous or unused reference geometry or sketches can be deleted toward the end of the modeling process.
Figure 3. Using reference geometry and initial sketches.
Primary features are features that make up the bulk of the overall shape of the model and would never be suppressed or removed from the design. These features must relate only to the reference geometry and initial sketches. Perhaps the most important rule for moving forward in the model is to never redefine anything that has already been defined in the initial sketches and reference geometry.
Figure 4. The role of primary features.
Primary features will typically consist of an initial base feature, plus up to a handful of other features that constitute the overall part profile of the model (see Figure 4).
Secondary features may relate to the initial reference geometry and base sketches, or to primary features (see Figure 5). To determine if a feature falls into the secondary feature category, ask yourself, “Would I ever want to suppress or remove from this from the design?” If the answer is yes, the feature is likely secondary. Secondary features typically include things like cutouts, pockets, holes and bosses.
Figure 5. Secondary features may relate to the initial reference geometry.
Detail features are features that you could easily suppress or remove to make a low detail version of the model. This includes threads, small fillets, chamfers and text (see Figure 6).
Figure 6. Detail features can be easily removed or suppressed.
Sticking to the Plan
It’s easy to have a plan—the real challenge is sticking to it when things get tough!
This modeling methodology hinges on two things: organization, and careful and selective use of references and relations.
I highly recommend the use of folders to help with organization.
Having the right type of features placed in their respective folders provides an inherent self-check to help ensure that you are conformant to the model plan. The folder structure also makes it manageable to navigate massive feature trees. Once you are comfortable with the standard process, you can deviate from such strict folder names to a method that works best for you.
While the shaft example has only 27 features (see Figure 7), a much longer feature tree doesn’t need to take up any more vertical space when using folders.
Figure 7. A shaft example with 27 features.
Some users may prefer to label individual sketches/features rather than use folders—another valid organization method.
Dynamic Reference Visualization can be enabled in SOLIDWORKS by right-clicking the top of the FeatureManager design tree as shown in Figure 8. This is a great tool to periodically check and ensure that your relations and dependencies are going according to plan.
Figure 8. Using the Dynamic Reference Visualization tool.
Once the Dynamic Reference Visualization tool is enabled, features automatically highlight their references, so you can quickly validate whether the dependencies are correct. As you can see in Figure 8, the primary feature points back to only base reference geometry, whereas features further down the tree in the details folder may point back to both secondary and primary features.
Unfortunately, it’s easy to pick up relations by accident! To help myself focus on relating as much as possible to my base sketches and geometry, there are two tricks I like to use. Both methods revolve around hiding the part display, so that it’s only possible to reference the initial sketches and reference geometry—you can’t easily pick up a relation to something you can’t see!
My preferred method when trying to avoid accidental relations is to hide the underlying body—either by right-clicking and choosing the eye icon to hide the body, or by using a shortcut to hide bodies. To do this, hover the mouse over the part and press the Tab key on your keyboard. Then, show the initial sketches and reference geometry that you want to reference. Add your features and once you are done, hover over the area where the part was and press Shift+Tab to show the body again (see Figure 9).
Figure 9. Hiding the underlying bodies to avoid accidentally picking up relations.
Adding features using this method will result in features being placed at the end of the feature tree, which can be freely reordered upstream at will since they will only have dependencies to your early base sketches and reference geometry.
If you do need to pick up a reference to existing geometry, you can quickly show the body again while modeling. The objective is not to completely avoid using references—secondary and detail features will inevitably need some references to other features. The objective is to put careful thought into what relations you add, and, for me, hiding the body forces me to really consider each decision—and ask, “Do I really need to show the body to pick up a reference, or do I have enough information in the base sketches/reference geometry?”
The second approach is to simply roll back in the feature tree to how it was before the initial features were created as shown in Figure 10. Sketches or features you create at this stage can then be reordered down the tree if desired. If you are using the suggested folder structure, it may be necessary to toggle to Flat Tree View (CTRL+T keyboard shortcut), which organizes features in strict chronological order—temporarily ignoring folder display.
Figure 10. Rolling back the feature tree.
The downside of the rollback bar approach is that there is no fast toggle in the event that you do need to reference existing features.
Another thing to watch out for is accidental defining parameters that are already defined in your initial sketches or reference geometry. Unfortunately, SOLIDWORKS makes it very easy to do this! A common offender is the “blind” end condition on an extrude or extrude cut, which adds an additional feature dimension. If it is being used for a primary feature, the length of the extrude should already be defined somewhere in your initial sketches or reference geometry. Using an alternate end condition such as “Up to Vertex” or “Up to Surface” allows you to reference a sketch point or plane, respectively.
This way of thinking is what will help prevent having only portions of your design updating during a model change—and it is worth taking the time to correct issues like this immediately as they are encountered to stay conformant to the modeling plan.
In summary, I recommend creating a hand sketch or model outline in advance of creating your CAD model. Establish the key parameters that will be driving the design and use those to construct initial sketches and reference geometry. Reference back to these sketches and reference geometry exclusively to define your primary features—don’t redefine any parameters!
Once you have created secondary features and detail features, try to reference back to the initial sketches and reference geometry as much as possible —hiding the body and showing these sketches is a useful trick to force this. Expect that you will need to show the body again to reference primary features with certain relations and create new sketches for your smaller details. Periodically check the Dynamic Reference Visualization tool and make sure that features don’t have excessive amounts of dependencies.
Planning a Project
Everything discussed so far pertains to individual part modeling, but if you are tasked with planning out a full project or assembly model, it’s worth doing some additional high-level planning. Below are my major considerations when approaching a new project.
Design Inspiration/Research
Design inspiration and research is a crucial step whether you are brainstorming a new idea or working within strict specifications, and I believe it’s always worth doing some healthy research and trying to create a design inspiration collage (as shown in Figure 11). I always gravitate toward Microsoft OneNote, where I paste in pictures of various design ideas and annotate the aspects that interest me.
Figure 11. Creating a design inspiration collage.
Hand Sketch and Preliminary Model
After choosing some parameters for my design, I return to paper to create hand sketches that will determine the overall structure of my assembly. Often it is also worth taking the time to build a preliminary concept CAD model, which can help you pick a winner from several competing designs (see Figure 12).
Figure 12. Building a preliminary CAD concept model to help choose a winning design.
These preliminary models provide a bare-bones level of detail— enough to get the information needed to make a decision on how to move forward.
When creating the hand sketch and/or preliminary model, start to think of the logical splits for parts and subassemblies as you move into tree structure planning.
Tree Structure Plan
Developing a tree structure or “design tree” before you embark on your detailed modeling can reduce a host of issues. It should certainly be a requirement for working in a collaborative environment, as the separation between subassemblies is what enables concurrent design. Only one person can have write access to the top-level assembly at a time (or any other part/component), so breaking up the model into logical subassemblies enables multiple users to be working on separate regions as shown in Figure 13.
Figure 13. Breaking up a model into subassemblies enables multiple users to work on separate areas.
SOLIDWORKS Treehouse is a stand-alone application that allows you to plan new assembly tree structures, and even create the necessary assemblies, subassemblies and part files associated with them. Treehouse isalso usefulforretroactively viewing an assembly tree structure. If you don’t have access to Treehouse, using Microsoft PowerPoint, Visio, or another similar flowchart tool can produce effective plans.
Model Requirements
After defining a tree structure, it’s important to define the purpose of the models and what their “inputs and outputs” need to be. This means establishing design requirements for subcomponents as you would typically do for a full design—perhaps using specifications obtained from your preliminary model.
Although it’s not always possible, ideally requirements would be specific enough that each component becomes decoupled (effectively a “black box”),which is the best-case scenario for collaboration. Having enough data from the preliminary model to be able to set a detailed requirement like “Motor subassembly must fit into a 50 mm x 50 mm x 75 mm bounding box, and mate with standard 4 x 100 mm bolt pattern.” This reduces back-and-forth questions between designers and allows more progress to be made before integration into top-level assembly is required.
Level of detail is another important parameter that should be established—for example, what are the models being used for? Purchased vendor parts may be represented with a very low level of detail, while models for photorendering or CNC manufacturing need additional attention.
If you’ve followed along the modeling methodology presented previously, then you should have the best of both worlds—an easy way to vary the level of detail of your models by controlling the suppression of your “detail” features.
Part Numbering
There are many methods and systems for part numbering and entire books have been written on the subject. As it pertains to CAD, it’s important to have a system tohelp ensure that files have unique identifiers and won’tget overwritten by other parts (see Figure 14).
Figure 14. Numbering parts according to a system can prevent files from being overwritten.
Here is one example system: use a descriptive part name during the preliminary design phase, and a reserved serialized number for release. This is useful because you may not be sure exactly how many parts are needed during the preliminary design phase, and is also an inherent way to differentiate prototype versus release files.
Sometime during the preliminary design phase and tree structure plan, reserve a sufficiently sized block of part numbers. This can be as simple as having a shared spreadsheet (shown in Figure 15) where users reserve ranges. It can be worth reserving some extra slots for parts that could be used for future revisions, upgrades or repairs.
Figure 15. Reserving extra part slots for later use.
Once the parts are ready to be released, rename the file with the reserved part number and convert the descriptive name into the part description. This is also a great time to fill out any other relevant file properties that may be useful on the bill of materials.
Note also that SOLIDWORKS PDM Professional supports automatically generated part numbering, which can streamline this manual process.
Project Timeline
The best laid plans won’t help if you don’t hit the deadline! For larger projects, it’s worth establishing a project timeline—usually as one of the first actions (see Figure 16). If you’re new to generating a timeline, you may not be sure what to realistically estimate. Thankfully, you can modify or “rebaseline” the timeline as you gain a more accurate picture of when you will likely be finished.
Figure 16. Establishing a project timeline.
The best part of using a project timeline is that when you are tasked with a new project, you’ll have a historical basis that will help you to make a much better estimate of how long the next project should take. It’s also a great tool for proving that additional resources are required. One of the most popular tools for project planning is Microsoft Project (which produces Gantt charts as shown in Figure 16), but even marking down some critical estimated dates on a calendar can do the trick!
Summary
This article presented an example modeling methodology, relevant SOLIDWORKS tips, and basic project planning techniques. Every industry is different with their own unique requirements, so please consider this as simply one of many valid possible approaches.
I believe the most important thing is to adopt some form of system for modeling and project planning. By employing a system or methodology, you will be able to track your progress and make incremental refinements and improvements in the future.
I hope this article and the processes outlined will give you something to fall back on and allow you to take the complexity out of history-based CAD! If you enjoyed this article and would like more detail, then I recommend that you check out the recorded version of the associated presentation.