You suppress one feature and everything underneath it gets suppressed. You cringe, a volcano erupts under the sea and five babies are born, slapped and all at once and named Llyod. Don’t you wish those ornery SolidWorks Features would just behave sometimes?
Well there just so happens to be, not one, but two single ways to make sure your features will always work for the configuration you need them in. What is it?? We could choke it up to ‘having a plan’ but that just won’t do. We need specifics and that’s what we’re about to drop on ya.
Now, if you use configurations, within the mayhem of part version creation and feature suppression, you’ll know creating features to work well with those configurations can be a fine art. Fortunately, there’s the FeatureManager and a nice little thing called history.
The history (stack of features) can cause some pain, but it can also allow you to manipulate and locate feature to work perfectly for what you need to show in each configuration. That’s a single thing, but not the two single things we need to focus on.
The two ways to set up features for making them more useful in configurations are…
Separation and Elimination
How to determine where to put features for configurations
Ahhhh, they go together like fine wine and dancing. Whether it’s to simplify complex models or show a process, being able to choose features for configurations can be tricky. If you ever think a feature may need to be controlled by a certain configuration, stick to the following.
Separation
Make sure the feature is created as a separate feature
Keep holes separate from extrudes. Keep fillets and radii out of sketches.
Elimination
Eliminate (or reduce) references from other feature
If you need to suppress a feature that helps locate a hole, you can either create a reference plane that both can use or reference the sketch plane or dimensions off another feature.
Looking into it deeper
We can keep those two things in mind when creating parts, but do you first figure out what features you need to control or what configurations you need?
For me, it makes more sense to set up configurations I’ll need. For example, if I need a “Simple” configuration, I know I need to be able to suppress certain features in order to simplify the part. If I need a “Manufacturing Process – Step 1″ I know I need to separate certain features from others.
What kind of Configurations do you need?
First determine what types of configurations you’ll be adding. Companies have different aspects of design, engineering and manufacturing they need to document. Thinking along these lines can help you figure out what configurations may be needed. Here’s some example of what you may need to create configurations for.
Configurations for:
- manufacturing phase
- drawing views
- assembly process
- simplicity
- version control
- material layup
I work with a standard set of generically named configurations. These are a few configurations that should work within any industry, organization or process that wants to get more out of configurations.
- Complete
- Drawing
- Simple
Complete – every feature shown
Drawing – only features shown that need to be visible on a drawing
Simple – a simplified version showing only basic features
It’s (usually) easy to know what features I’ll have in these configurations, but occasionally some more thought will need to be applied, like knowing exactly what relations to create? Sometime you need one feature to define another feature. In this case you may need to use or create a base feature (plane, axis, or sketch) that multiple features can reference without being tied to one another.
When it Doesn’t work out
Occasionally, you’ll have those times where features were created together or get suppressed because they relate to another item being suppressed. In those instances, you can do a couple things.
- Change the defining sketch to construction and use it to locate new features
- Redefine a sketch plane or sketch relation by setting up new features
I will hardly ever just delete a feature and start over. It pretty easy to see where features are defined. To see where features have relations there’s also a couple things you can do.
- Drag the feature in the FeatureManager tree and see what feature you can’t move it past
- Delete a defining features and see which features get error (quickly undo after – Ctrl-Z)
How do you control your feature for use in Configurations?
There’s other ways, much depending on what product your creating or what the data needs to do. Feature dependency and sketch relations are just two aspects of what configurations states rely on, but probably one of the most important to understand and master.
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{ 4 comments }
Great article, i use configurations pretty much all the time, be it in assemblies or in parts themselves. I agree with every point you made actually, but there some little things i do that goes further than that i guess.
First i always make a rule of separating core features (extrudes, cuts, loft, etc) at the top of the tree, then drafts (i mostly do molded parts), then at the very bottom i will put every radii.
Radii at the bottom for 2 reasons, first they are the ones being pushed around the most, so i can rollback them all, do my stuff and then edit them at the end (using the last revision as a reference) and when sending a part to FEA engineers, they usualy dont require any radius, so i can just suppress them all without affecting the model.
You can also have them in batch for each revisions, it's easier when they are at the end.
Your point about using reference planes is a good one, although i might add that you can specify the plane of any sketch specific to any configuration, it takes a little planning but in the end you have less stuff in your tree.
When doing aluminium extrusions, i like to have every manufactured lenght as a configuration, so i don't have multiple parts each having the same basic sketch (which would be a pain to update…). For that i will link the extrude feature lenght to different configurations, you can do this by double-clicking the feature on the model, the extrude lenght usually appears as a blue dimension, you can then edit its value as you would a sketch dimension.
If you have cutouts that needs to be driven by the extrude lenght, you just add a reference sketch, or plane, that is linked to that extrusion lenght value, and everything follows accordingly.
You can also use the linear pattern in 2 ways for that one:
1. If you have one cutout that moves at each config, link the pattern lenght to the extrude lenght.
2. If you have a serie of patterned holes, i make a linear pattern for each config, and name it with the config name. That way i only have the first hole as a feature, for every configurations.
The “delete feature to see what will disappear” is a good one, i use it all the time.
Maybe you knew all this, but you didn't mention them so i thought i could add meat to an already nice article, or just real life scenarios
. If i think of anything else i'll let you know.
It's a nice and necessary article. Most of the beginers are struggling in this area.
I like (and used it heavily) the 'base features' concept in my models. Ususally I have listed all base features in the top of the feature tree with proper grouping. ? In fact all the dimensions are relations of the features are only being controlled by the base features.
Advantages I could see over this method are,
1. Extream freedom to control the features.
2. Profile dimensions are controled in one place (Use derived sketchs to avoid
equiations or link values)
3. Performance of in-context assembly is extreme good (most of the time equal to bottom up method) because there are no solid features of different parts created/controled by in-context. Only 'base features' are linked.
Disadvantages are,
1. In a regular SW part, we can see the related dimensions just by double click the feature, but in 'Base Features' method I couldnot see the dimensions because it refers to other base sketch/plane. This is difficult for a another person who will maintain this features. Eventhoug the base features are relatively named and propoerly structured, sometime I myself suppose to use 'Parent Child' relation functionality to identify the feature dimensions.
Yeah, I see your point on the disadvantage you talk about. I run across this with top-down models that use a reference sketch that hold all the dimension. People will inherently look for the dims in the feature, but everything is in another sketch, maybe not even part of the model.
This is where 3d modeling can get really complicated and where it important to explain how it's done instead of assuming someone will be familiar with modeling that way.
Thanks for bringing that up JRat!
Yeah, I see your point on the disadvantage you talk about. I run across this with top-down models that use a reference sketch that hold all the dimension. People will inherently look for the dims in the feature, but everything is in another sketch, maybe not even part of the model.
This is where 3d modeling can get really complicated and where it important to explain how it's done instead of assuming someone will be familiar with modeling that way.
Thanks for bringing that up JRat!
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