So, you're a sloppy modeler and you don't organize your model tree in a way that makes sense in the future?
In the immortal words of Bob Newhart:
Seriously, though, only you know what your models are like and how you have to interact with them in the future. You are in the best position to take some time to plan things up front, name things well, organize them into folders, etc. to fit with your workflow.
Here's a few things I try to do as I go.
Name all my sketches and planes. I use sketches and planes to apply mates to. Once I create one, I give it a descriptive name. (Often I can make my parts reference those sketches so if I change the sketch the parts auto-update.)
Move sketches and planes to the top of the tree as soon as I make them. This reduces circular references and its easier to find the right sketch if you don't have to hunt for it in a long tree of items.
Similar types of parts get moved into a folder and the folder named for easy reference.
Name any patterns that I use as well.
As Joe said, name sketches, planes, and patterns. I also name features if there are more than a few, and seeing some of your models here you certainly have more than a few. It's also helpful to group related sketches, planes, features, and patterns in folders (as long as they are only used by other features in the same folder) and name the folders.
And this probably won't apply to you, but I've often seen other people's models that have reference planes that they don't really need.
In addition to the great suggestions you received, let me add one:
Take advantage of the new Favorites Folder functionality:
I guess naming would be one solution but I was thinking of a grouping type of thing. Here is the real problem. If you move all the reference sketches and planes and sufraces to top then once you supras a certain point 100+ featurs if you have to go back to change something then entire tree has to reload in order to gain access to that reference geometry at the top. So thats the real bummer. I guess I try to use folders and names
One thing I try to do is get a good idea of how I will model something before I start. That way I don't trip over myself too much, and make a mess. I don't rename features too much, but I do put them in folders to be neat if I have more than a dozen, or so.
It is largely going to depend on your modeling style and type of designs: I don't end up having many sketches visible in my feature manager as they get absorbed into features. I rename the features to simplify revision when warranted, and group features into folders based on function or location.
Like Andrew stated, having a plan before you start helps, and when you realize your perspective needs to change it can be good to regroup from that point. It is more frustrating to fight with a model repeatedly than to admit you need to do some housekeeping to make it easier to continue working in.
Chris, have you tried the "Flat Tree View" in order to see the sketches unabsorbed in a historical manner?
Alin - I prefer the sketches being consumed just to keep things tidy. With the features named I know which one will contain the sketch I'm looking for if I need to reference it.
But I'm in the dim ages (limited to SW2011) - when was flat tree view added? I've never seen anything remotely like that and every entry in SW help for "flat tree view feature manager" is all about sheetmetal flat-pattern.
With Andi saying 200 boundary surfaces I can see it getting tedious. I work almost exclusively in solids so my current worst part is 172 features.
Aha, that explains it. SW 2013 and 2014 introduced a few more options for managing the feature tree. Little goodies like:
- favorites folder
- history holder
- flat tree view
I think that Parent / Child functionality is the good way to quickly find right feature. I never name or group features, at the end, that never helped me so much.
But it also depends on complexity and type of parts you are doing.
Its great when you drawings and know how end result will be but when you model and improvise as you go along then complexity and design tree grows and grows and grows next thing you know you have 200 boundary surfaces
Naming is essential on parts with a large number of features, but I use folders a lot to group by function, especially of surface operations. It make it a lot easier to locate things wiithout extensive scrolling. Oh, yeah--and name your folders.
A. Use folders!
2. Name key features!
I like layout sketches. Helps in building a robust model that stands up to changes over time.
Make every model with the idea that it WILL change. You (or some other unfortunate) will have to go back and change things, long after the heat of battle is over.
Get in the habit of doing things right, and soon the right way will be faster than the "fast way". Especially true later in a model's life. That's when having done things the "fast way" will really slow you down.
I too like to use Layout Sketches but I also use them at the part level. I basically layout as much of the part I can on the 3 cardinal planes, so I end up with a “Right Sketch”, “Top Sketch” and “Front Sketch” (each with its own color). Included is not only the basic geometry but also points that control the location of planes, axes and etc. I will need in the future. I then create said planes, etc. and put everything in a folder at the top of the tree. As I construct the model, I then relate the feature sketches (the ones that get absorbed) to the cardinal ones. This takes a little extra time up front but as the design evolves all I need to do (most of the time) is go to those 3 sketches and make the appropriate changes. If I find I need more references, I will roll back, add them to the sketches and then roll forward again. It has been my experience that I spend more time editing models than building them so for my workflow this, in the end, saves me time.
PS… I agree with most of all the other suggestions.
Love the different color idea. So simple but I never thought to change them.
Start with three reference sketches; one on each default plane.
Every subsequent sketch should have very few dimensioned features or relations; it should be filled with converted entities. Remember, Solidworks is your enemy and will use any excuse to fail a rebuild. NEVER reference to a piece of 3D geometry. NEVER reference to a sketch not among the three reference sketches.
Sketch planes should be either (a) one of the default planes, or (b) a plane created by features in the reference sketches. Remember, Solidworks is your enemy and will use any excuse to fail a rebuild. NEVER choose a face on a feature for a sketch plane.
Features such as bosses and cuts should go from one vertex in a reference sketch to another. NEVER use "through all" or "blind" or (god forbid) "Up to surface". Remember, Solidworks is your enemy and will use any excuse to fail a rebuild.
Done right, you will have a part with a minimum number of features that all reference ONLY to one or two reference planes. Remember, Solidworks is your enemy and will use any excuse to fail a rebuild. The more nested your references are, the more chance things will break.
Finally, NEVER use (a) external references, (b) 3D sketches, or (c) sheet metal. These aren't features; they're actually pranks Dessault are playing on users.
Couple of things I do to keep large feature trees manageable
I'll skip naming features and creating folders since that bells been rung-but do it.
1) for machined parts, unless design requirements say otherwise, I model in this order
base feature, large bosses, large cuts, small bosses, small cuts, ribs, drafts, lage fillets and chamfers, machined holes, small fillets and chamfers.
2) for molded plastic parts:
base feature, shaping features, pockets, shell, ports, thru-holes, parting features, lips, grooves, core side mounting features, cavity side mounting features, capture features, webs, ribs, drafts, core fillets, cavity fillets
3) work systematically from general to specific. Big features near the top of the tree, small features near the bottom. When I put in stiffening ribs on a plastic part, I put them all in at once and keep them together. When I'm putting holes on a flange, I do all of the holes on that flange and avoid jumping around.
4) work in one locality at a time. think of your design in terms of functional areas. Do as much as you can on the bottom of your part before switching to the top. When I had to make a mounting plate for an electronics assembly I had power supply features, magnetic switch features, ballast features and lamp features so that when I picked on one feature, I had a good idea of where the other features were.
5) clean up after your laziness: there's nothing that says you have to get your organization perfect as you build the part. But when you get a breather on a large part, where you're trying to decide what to tackle next, move features into groups, consolidate patterned features, name your features, put things into folders.
6) don't beat yourself up about the number of construction features or layout sketches you have. Sketches and reference geometry are very stable and usually build faster than solid features. Give them names and stick them in folders if you don't have a downstream use for them. Get creative with naming: its' good practice for designers to say, what does this feature provide that no other feature does? Hint, if you can't answer the question, you've spotted an opportunity to improve efficiency and eliminate redundancy