Better to have multiple simple features, or 1 complex feature?

Performance wise, I don't know - I have never tried to test it. I do know that simple sketches work better than complex ones, but where that point is, I don't know.

I think what will make a bigger difference is doing it like you do. It is a bit more organized as you can name the features accordingly, you can suppress certain ones for different configs, and you can populate hardware with feature patterns, rather than manually.

WT

Hi Monkey -

Heart felt rules for myself-

- 1 sketch for everything if possible: it allows me to adjust the whole mess from one point. I have even taken this to draw "phantoms" in one sketch and convert them in a subsequent feature to make the feature supressable, but to have both features controlled by a single sketch. This, for me, is a very valuable thing - maybe not for others. I usually also do all fillets in a sketch - perhaps bad in other ciscumstances.

- Holes are always made by the hole wizard. My only exception to this is when I know for sure that I only need one hole and will not ever need two of a certain size - also on revolved parts - the center is always part of the base revolve. Having patterns helps me when patterning hardware in assemblies later.

- Sketch patterns when not too big, but external patterns when they get big - supressible.

- Supressible features if showing a progression is needed for machining or forming.

I always try for the tightest feature tree - it's a little bit of an obsession, but a needful one for me. Most of my parts are prismatic solids - no splines or surfaces.

For what it's worth. Do what makes the best for you - no two working styles are the same and sometimes mixing styles is a problem.

Later,

SMA

Avoid complex sketches. Rule of thumb: if you're struggling to make a sketch work you should be doing it with more than one feature.

Sketches are dumb. Features are smart. Don't do a revolved cut for a hole, use the hole feature. You'll also benefit when you go to do the drawing, you'll get a hole callout if you use a hole feature, etc. etc. Also, don't sketch fillets unless you have to. Seperate features can be reordered, supressed, or easily modified, they have properties specific to their just their feature type.

Overall you should strive to have a short well ordered model tree, but at the same time you should not try to do everything with one or two features.

Layout sketches are very helpful too. And if you're smart you can reuse sketches for several features, especially by selecting contours.

On top that use folders to organize related features. Always name your features and sketches, with descriptions if possible.

I can't say for sure in SolidWorks but in Pro/E using the approriate feature for every aspect of your model decreases regeneration time.

As per your holes, I'd use the hole wizard and a sketch pattern for each set. Then put them in a folder that identifies what they mount to.

OT: why doesn't SW have derived feature patterns? In Pro/E they are called reference patterns. I used to define a hole patern(s) in a mold plate and then do a reference pattern in the mating plate(s). It was great b/c all my holes were tied together and all I had to (re)design was the mold plate.

I dont see why you would not be able to do this. At the Assembly level, you could make a component/feature pattern and base it off the other part file so that if the one changes they both do.

"SW Monkey" wrote in news: snipped-for-privacy@g43g2000cwa.googlegroups.com:

Others have hit on some good points. I'll just add my votes for a few of them.

- Simple sketches. Complex sketches fail easily when changed and take a long time to regenerate.

- Sketch fillets are notorious for busting up the sketch when things change. Plus, if you want to get rid of them it's a real pain. Use feature fillets unless you absolutely have to use a sketch fillet.

- Definitely try to use patterns. SW has some nice ways to pattern stuff. Don't overlook the sketch driven pattern (feature position driven by a bunch of points). The hole wizard pattern with multiple points works just like the sketch driven pattern. Remember that for the Hole Wiz, by default the pattern sketch is a 3D sketch and you can pattern holes to faces other than the first face, and the holes will all be normal to the faces they are placed on, including on non-planar faces.

- Using the sketch "step and repeat" patterns always kills speed. I avoid this like the plague.

- If you have a single fillet feature with 100 edges selected, it is faster than having 100 fillet features with 1 edge selected. Of course this is assuming that the two would give you equivalent geometry.

matt

Another thing that might be useful is the Feature Statistics, if speed is an issue.

I played around with this a bit and it can tell you where your "fattest" features are.

I made a simple model with Sketched Vs. Feature Fillets and found that they took an identical amount of time. My example was simple, but it should tell us what techniques are bad or good (performance wise).

I think that the problem that comes in is when someone really goes at modeling in a round about way - there are many stylistic differences and I simply say "it's not what I would have done, but it's not wrong either" - other times you just shake your head and know that it is wrong - no discussions. I have seen point sketches premade for hole wizard features right on top of the pre-sketched points in a subsequent sketch. Some seem to only start any model with a cube and whittle away at it as if they we doing machining. I have seen people mate a hundred screws in an assembly seemingly unaware that patterning is even an option, not even using mate reference for screws - like it's easier to do it the "easy way" than to force ourselves to learn anything new.

In any case, the feature statistic tool will be a fine helper if one lets it.

Later,

SMA

(Slightly OT: I also wanted to mention that anyone who uses google to read mail might really like their new toolbar - it spell checks when you post or in any other web form. Take a look if you use google - its nice)

Unfortunately, your question may not have a simple answer since its probably varies from case to case. Nonetheless, I will offer my observations.

Generally, I prefer to not get too complex with each feature to make future editing more manageable, particularly if someone else is editing my projects. On the other hand, I do leverage some of the tools in SolidWorks to speed up design. Talking about holes, I will sometimes create several sets of holes in a single feature - particularly if they are somehow related. I try to avoid creating so many holes in a single feature that the sketch gets hard to understand. For example, I would hate to edit a single sketch that defined the position of 100 holes with X-Y coordinates.

Having said that, I have seen indications that more complex features offer improved performance. I should state that these observations were made in SolidWorks 2004 and I haven't repeated the following tests in 2005. Our local users group had one evening in which everyone was invited to model the same part using their preferred method. During the meeting, we reviewed each model looking at construction techniques, degree of complexity, and rebuild time. The fastest rebuild times were associated with the parts built using the most complex sketches and features. For example, the inclusion of sketch fillets was better than adding fillets as separate features. This result came as a surprise to many of us in attendance. It would be very interesting to repeat this experiment using 2005.

Is anyone interested in participating in such an experiment? This could be done in an online version to look at performance issues and the submitted models could be posted on a web site for download and review.

As far as I can tell you cannot use a feature pattern to drive another feature pattern.

You can use a feature pattern to drive a component pattern, but that's it.

I think that this would be a fun thing to do and a great way to talk directly about modeling practices, everyone would probaly learn something. Any suggestions on what would be a good part to model?

In my opinion, just about any part that has a variety of features would be interesting. I definitely would include some fillets and possibly at least one rotational feature.

This reminded me of a challenge they were always having on the inventor discussion. Go to

is a monthly challenge to quickly and accurately model a part. It is mainly designed to challenge inventor users, but could also be done by SW users. It would be a good head to head competition of Inventor vs. SW

Brian

John Eric Volt> In my opinion, just about any part that has a variety of features would be

I went to the following web site, but its unclear how someone participates. Can you point me to a page with contact and sign-up information?

I just took some time to perform some simple tests in SolidWorks 2005. I created a rectangular block with four filleted edges so that I could create it using sketch fillets in the extrude sketch or by adding fillets as a separate feature. Here are the results as determined with Feature Statistics:

Extrude the block and add fillets as a separate feature - 0.06 seconds

Extrude a filleted block with sketch fillets in the sketch - 0.03 seconds

Apparently, using a more complex sketch is more efficient (by a factor of 2) than having a separate feature for adding fillets in this situation.

I also created a cylindrical part with fillets on the ends by rotating a rectangular sketch and adding the fillets as a second feature. Additionally, I created the same part using a single revolve feature that incorporated the fillets in the sketch. Here are the results from Feature Statistics:

Revolve a rectangular sketch and add fillets as a separate feature - 0.01 seconds

Revolve a filleted rectangular sketch - 0.03 seconds

In this case, the more complex sketch requiring a single feature has a much longer rebuild time.

Although all of these times are very short and the difference would be undetectable when hitting rebuild, such a difference is quite informative and may prove to be very important when working on more complex parts. Unfortunately, the cause of the differenes between these cases is unclear and additional testing/research would be required to determine the most efficient approach to modeling various parts.

If I have some more spare time, I will do some more experiments in the future and report back to the group.

I was wondering about the inconsistent results I reported a few minutes ago, so I went back and reviewed the Feature Statistics again. Upon reviewing everything a second time, the 0.01 second rebuild time I reported for revolving a rectangular sketch and adding fillets as a separate feature is incorrect. SolidWorks is now giving me a rebuild time of 0.03 seconds. Its possible that I mis-read the result the first time. Nonetheless, adding fillets as a separate feature no longer improves the efficiency in my test cases.

Until you want to remove the fillets or apply draft to the part or do a pattern or make changes that cause the sketch fillets to fail.

A couple of years ago I did a test for patterning. The results are still around on my site.

go to Rules of Thumb, then Patterns.

You could try either a derived sketch (and sketch based patterns), or the hole series (in hole wizard).

Both have worked for different cases in the past for me...

Really complex sketches take longer to solve. They can be a bear to maintain also. I leave fillets to the fillet feature.

I do use sketches in contour mode so that design intent can be carried across multiple features. Even if the sketch is a little more complicated it is only solved once.

Pattern features not sketch elements if possible.

Grouping holes by size in a sketch makes sense. Using hole wizard for this also makes sense. The downside of grouping holes in separate sketches is when making a drawing with imported dimensions.

I have communicated with the guy who runs the Inventor World Cup and there are no SolidWorks entries. I suspect that they really aren't setup to judge SolidWorks entries, though. Therefore, I would suggest starting a similar contest for SolidWorks users. I would be happy to help setup such an activity, but I would like to know if there is any interest among the SolidWorks users. Any thoughts?

SolidWorks has held Design Contests from time to time. Cosmos has also done this. So has PTC. Tenlinks was involved with a SW / Inventor Shootout a while back. It didn't do much for the credibility of those that held it because it didn't have the support of one of the competitors.