Cover your hair. We are firing up the burners on the Feature furnace of SolidWorks about to drop some gas-drenched geometry into the flames.
There’s a slew of Features that thrive on 3D geometry alone, but I’m not gonna say, “You, go learn about Features!” eight times. Post like that are useless and annoying. This is to show you that modeling in SolidWorks isn’t all sketches. We’ll look at eight guideline and the reasons why they’re gonna make your 3D sizzle.
The more I model parts and assemblies in SolidWorks, the more I find I want to get away from sketches. Not because they don’t work. The sketch features in SolidWork are incredible and gain more functionality each release. (Yes, I really believe that.) I want to work with the 3D geometry, because it keeps me in the context of the 3D part geometry. I don’t want to do extra work to stay there, so there’s a group of guidelines I use for creating feature-based geometry. Here they are.
- Create the basic solid without any holes or radii
Reason: You’re able to use edges and faces (instead of sketch lines and planes) to define features added later.This also gives you more leverage over features. Creating them after the basic solid allows you to control them via configurations, move them around in the FeatureManager and gives you more options for feature appearance and control through the application programming interface (API).
- Use the Hole Wizard for any Holes
Reason: For the same reasons above, this gives you leverage over Hole features.It also allows you to change standard Hole sizes more quickly, pattern components easily with a Feature-driven pattern, and they can be created in both parts and assemblies to drive SmartFastener Features.
- Use surfaces to control features
Reason: Surfaces can be created quickly from existing geometry.Extruded and revolved surfaces require sketches, but many of the other surfacing features can be used with existing geometry, even solids. Surface don’t add volume (weight) and can be hidden easily. For example, you can define cutting planes with a mid-surface or radiate a face to define other features.
- Use solid geometry to define reference geometry
Reason: Allows another dimension of definitionInstead of setting up more planes and 3D sketches, use faces, vertices and edges to create reference planes, an axis or coordinate systems. For example, you can right-click and select the midpoint of an edge to define the location of a plane.
- Use features to define and end condition
Reason: Allows new feature to change with other changes in geometryIf you use a face to create an ‘Up to Surface‘ or ‘Up to Next‘ condition you’re building intelligence into your model and allowing it to adapt to changes in your design. For example, if you locate a support rod in a sheet metal enclosure, defining its length from face to face updates it if the size of the enclosure is changed.
- Locate new features off faces/edges least likely to change
Reason: This will reduce the amount of editing and error fixing you will have to doBy defining (guessing) what edge or face may change the least, you set up a process of creating new feature. For example, you may know that the CNC operator always starts from the lower right-hand corner. You set those edges and faces as the points where features will be define from (with respect to designing the part for change).
- Use Planes to create Split lines and to drive other features
Reason: Planes can be defined with existing features and split lines can create edges and vertices not possible with a single 2D sketchSplit lines in themselves can be utilized for creating reference geometry and build features. For example, you can split the face of a sheet metal part to define a rip or radiate a surface to trim a flange against.
- Move/Copy Body
Reason: Keeps you from duplicating sketches and workThis very simply copies/moves a feature you’ve already creat. It reduces rework and makes it quicker to add geometry. For example, you may have some gussets along a weldment. You can copy the bodies to specific locations without having to recreate sketches or add extra cuts.
The disadvantage…3rd degree burns and lost references.
Feature-based modeling makes geometry creation really enjoyable. The disadvantage of defining features by other features, however, can cause some real discomfort. If you delete (or change) an edge or face, you can get errors telling you that a feature is undefined. Even though this takes time to fix, You have control over that feature. You’ll have to go into the sketches of course, but therein lies the advantage of a sketch-based, history-based system – you have more freedom to control features when there are changes.
Ok, so go learn about Features. I kid. But really, setting up some basic guideline for how to used them goes a long way toward getting those features to work better in SolidWorks. Is there anything you want to go into deeper with this? Do you have your own tricks that makes modeling with solids less sketchy and more useful?
Loading ...
SolidSmack is a very small behemoth of an online community about 3D CAD, technology, design, robots, and ninjas… Ok, maybe not ninjas so much, but those guys are COOL so there just might be something about some dang ninjas.
{ 12 comments }
I see the opportunity for an additional article on feature-based modeling for configurations. Knowing what features are unlikely to change for multiple or future configurations is a talent. When I suppress a feature for a new configuration and all the linked features suppress, I am routinely impressed/annoyed with myself.
Alright you got me, the rest of the day I am going to attempt to ignite something and use Feature-based Modeling.
Let me know how it goes. there's lots of things you can do if you think, now, how can I do this without a sketch? Is it easier? or quicker?
Have fun!
OOO, no kiddin. This would be good. I'll see what I can whip together. I think it helps mostly to know what configurations you'll be creating. I use a standard set, but I've had times when someone will come to me asking for a configuration of _____ and I have to rework how some features are referenced. uhhg.
Josh,
I agree with first two guidelines, but not sure about the rest of them.
Let me see:
Using features and faces (3,4,5) to define other features or boundary conditions for them might be a very quick way to build models, but a certain one to the headaches, especially for complex parts or for parts with many configs. I've learned to rely on equations,relations and layouts, for both assemblies and parts. Sooner or later, your model will be shared with an mate/colleague or with other guy, even on different CAD system and updating such model will be a nightmare. We frequently receive CAD models from suppliers or from clients build as you said and the update/change process is a difficult and time consuming one.
But, as exercise for beginners, for simple models or for models that will never go to the FEA analysis and will never be exported in another CAD format to be used by others, it's fine.
6. This is a tricky one since you will never guess the future of anything.
7. Useful for sheetmetal or for die cores, but useless (for me at least) for other, since you can use the plane itself as reference, or “Intersection Curve” (between that plane and desired surfaces) inside of the sketch, without making another feature (the split line).
8. This is tricky also. You should be so careful with these! And they are difficult to change if you use constrains instead of dimensions. For intensive usage of the same body, I would made an user Library feature part. It's a little work to do Library parts but it's worth.
When i use Configurations, i always rename the features related to each in my tree. Something like Cut-Extrude1_Cfg02, Cut-Extrude1_Cfg03. Even keeping the same feature number if its used on multiple configurations. That way i know what goes where, no questions asked. There are tons of stuff to consider though, can get overwhelming in a big part.
ok, 25% in agreement. I'll take that
I somewhat agree. This is a little exploration into creating features with fewer sketches and some ways I've used it to create some, yep, in a collaborative work environment. I'll try to explain a little better.
First with any feature, it's good to name them, give the context. The features in theFM can be a confusing heap of a list no matter what the methodology. I really like using 3 and 4. number 5 is hard for me because I come from a sketch-driven assembly background, but with multi-body parts and being more disciplined about what references I choose makes this a more enjoyable modeling experience.
I can't reinforce enough how important it is to keep references contained to one area, whether it's sketches or features. I will have either a 'Driving Sketch' or 'Driving Body' part (sometimes an assembly) that I keep reference to. This becomes really useful when having to maintain consistencies across multiple assemblies.
anyway, not to get too far off.
6. I'll keep reference to a 'corner' of an assembly and often the center of a part.
7. I like this because I can split multiple faces to get some edges to work with. Sometimes a plane just won't 'cut it' (har har)
8. I've used these a lot more with multi-body modeling. It definitely needs to be laid out in a method or sorts if someone in a company thinks it's an efficient way to model.
Really, it a good idea for a company or group to determine best practices for what they're designing. Some of these won't be the best way, especially if the shop needs certain data. (multibodies are not good if the shop needs parts broken out with defined properties.)
I see where you're coming from. I think it's interesting to get into some areas that are not often thought of in our highly sketch-driven world of solidworks.
Thanks for the great comment!
Wow man, that would be tedious it seems. That would be cool if it happened automatically, or if there was an option to append config name to feature. now we're talkin!
Well, as i always like to say, i prefer taking the extra time at the start of a modeling job and prevent losing hours in the middle and end of it, trying to figure out what goes where. I am talking about intensive config use though, i could maybe try and send you a file or two so you get the idea. In the best case scenario, you can split your tree in 2 or 3 folders, each one containing a batch of config specific features, but it rarely is that simple
Josh,
Sorry for my aggressive comments. Even in my culture they said that I'm too direct, if not rude.
We are working especially for big American clients, so I'm familiar with ANSI, ASME and clients specs and needs. Because such a diversity of projects and CAD platforms : from simple conversion 2D to 3D few years ago, to entire industrial programs with few years duration, from Inventor,CATIA, SolidWorks,UG-NX to Pro/E, learning each from other, we have established some internal best practices for each platform and project type. And my comments are in line with this practices.
But, of course, I would like too see others comments, especially from those who doesn't work in a mechanical area: sculptors, RP artists, designers, etc.
Again, my apologies for the comments tone.
I think you made a great job here. I would like to be in your skin
Hey man, not aggressive at all! I appreciate the comments for sure. I think we all come from different backgrounds and there's a lot of modeling techniques that work better in each person's field. I wouldn't want to discount anyone's ideas. It helps me to take a second look and sometimes find better or different ways of modeling something. so , thanks! and keep 'em comin!
Hey man, not aggressive at all! I appreciate the comments for sure. I think we all come from different backgrounds and there's a lot of modeling techniques that work better in each person's field. I wouldn't want to discount anyone's ideas. It helps me to take a second look and sometimes find better or different ways of modeling something. so , thanks! and keep 'em comin!
Comments on this entry are closed.
{ 1 trackback }