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eobet

Why Does Solidworks Do @#$@#$ Like This?

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I'm modeling a car in 3D and it's the biggest project I've done yet, with over 100 sketches and 200 features.

 

Here's some quirks I've encountered:

 

1. After mirroring half of the surface model and stitching it together into a solid, and then going back in history to have a look at the surfaces again, Solidworks reports that it can no longer stitch it back into a solid, even though I did not do anything to the model! I just looked.

 

2. After moving a curve at one end of the model, a feature breaks on the complete other side of it. The feature claims that it can no longer convert an entity, which is a projection of an edge. I try to delete the curve and then convert it again, but it refuses to convert, even though I've done it before and the edge hasn't changed. However, if I just delete the relation, and keep the old converted curve, the feature will still do exactly what it did before, without breaking.

 

3. After moving a curve at one end of the model, a feature breaks on the complete other side of it. This feature claims that it can no longer merge two surfaces in a mutual trim, even though they haven't changed. I am forced to do two single trims and one stitch, in order to do exactly what it did before.

 

4. I've projected several straight line sketches onto surfaces to create split lines. I want to sweep cut with that line, but Solidworks refuses, because the line isn't XXX. However, if I sweep cut each segment at a time, it works. So, I know Solidworks original claim is bullshit.

 

5. I've built a boundary surface and then split a line across it, in order to be able to draw a curvature continuos spline from its edge. However, sometimes it works, and sometimes it gets over-defined (how it can get over-defined just from selecting the curvature relation on a spline in a 3D sketch is beyond me). There is no pattern to this. Further, sometimes I can convert the split line into the 3D sketch, but then the curvature continuos spline freezes and looses its editing capabilities.

 

I love that Solidworks is parametric, but I hate it when it breaks for no obvious reason.

 

I love that Solidworks is finally able to do curvature continuos stuff, but I hate that it's so limited.

 

EDIT: Attached a nice little screenshot of two split lines across a single boundary surface. Notice the grey 3D sketch in the background? That's a curvature continuos spline attached to the split line of that surface. Notice the RED sketch in the foreground? That's a curvature continuos spline attached to another split line of that surface. Both split lines are straight lines projected from the top plane. WHAT ON EARTH MAKES SOLIDWORKS BEHAVE THIS WAY???

 

EDIT 2: Btw, that cyan line? I have no idea. It's not a split line, sketch or anything. It just appeared after the surface was re-built the last time.

post-526-1264016008.jpg

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Guest bildder

I understand you, I encountered similar problems many times, then I hate SolidWorks.

i.e. I have got a surface model (200 features), save it, and open next, after rebulid - failure...

rollbar moved up and program detects error. I force rebuild CTRL+Q, and everything is ok.

 

But sometimes I can't resolve problem, then usually I have to break references (save model as parasolid, and insert part into part) - I hate this workaround but I can't wait...

 

As for your question.

Have a look at picture below, you needn't create extra edge by using split feature (since SW 2008) /what's new 2008 /

 

post-16124-1264079706.jpg

 

BTW.

My last hybrid model is over 1000 features and file size is about 200MB...

 

post-16124-1264079889.jpg

 

Good luck with your work :)

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You're right about the constraints being hard to anticipate, sometimes they work and other times they do not. Remember though that you can always turn on curvature combs inside a sketch when right-clicking your spline(s) and you can match that to be curvature. It's the more manual, direct approach but sometimes it's easier when modeling complex shapes and forms.

 

It's true that the parametric nature of a program, any programs, is a fragile bonus once you get to a substantial feature count. However just rolling back and then forward again breaking things is of course unacceptable. I have had that with an earlier model but not with more recent models which tally 500-1000 features.

 

As hidden as it is, make sure to check out this very cool video from Mark Biasotti (from Solidworks) on how to add tangencies and curvature constraints without having to split lines first!!: https://forum.solidworks.com/message/46805#46805

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what year of solidworks are you running? I have found that 2009 seems to be much better than previous versions for surfacing and working with 3d splines in particular.

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Guest under-dog

Any time parametrics are involved things can get a bit quircky.

 

How the file is set up will greatly affect this. Things may "appear" to have been setup ok but there are certain relationships thay may hve been missed added or miappropriated that can cause failures when things get changed.

 

As far as the fine at first but fails on a rebuild. Sometimes there are little quirks and from what i have been told that when solid works does its standard rebuild or you press the little rebuild icon(stop light) it is just a soft rebuild.

 

contrl Q is a thorough rebuild. Every so often I will do this, especially if I have been josteling things around a lot and maybe doing some questionable operations. This will usually root out any underlying issues that the soft rebuild does not.

 

Even then though sometimes problems will root out on a soft rebuild.

 

Also keep in mind that in addition to being parametric it is also primarily what is called a solid modeler. It will do surfacing but IMHO this is a very shaky way to build a model but creating surfaces and stitching the sheets together at the end. At least in SW due to the parametrics. Oversized surfaces trimmed down are better and solids with surface trimming tools seems to be even more stable.

 

There are quirks but questionable "non-robust" build techniques are usually the culprit.

 

Just IMHO.

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when solid works does its standard rebuild or you press the little rebuild icon(stop light) it is just a soft rebuild.

 

contrl Q is a thorough rebuild. Every so often I will do this, especially if I have been josteling things around a lot and maybe doing some questionable operations. This will usually root out any underlying issues that the soft rebuild does not.

 

Very good point, I had nearly forgotten about this, but it's absolutely a good thing to work into your workflow after every 50 or so features.

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Eobert,

 

Let's take it from the top and work our way down...

 

1) As mentioned by under dog, Control-Q cannot be stressed enough. But for the best results make sure "Verification on Rebuild" is turned on in "Tools, Options, System Options tab, Performance". This may make your rebuild time slower, but it makes sure that 100% is on point with your model.

 

2) Mirroring, in general has it's place, but use it to mirror the door, the wheels, the lights. I would never suggest mirroring for the hood, the bumper, the windshield, the roof. You're just asking for there to be a seam even when the surfaces are knit. It's just the nature of the beast.

 

3) Don't forget that you can always "overbuild". Meaning take the surfaces past the point where you want them to be and then trim back exactly where you need them to be. Take a look at this model "Efebo Seat" as a good example. It can be found here www.ragde3d.com/free_dowmload.html

 

4) Though converting entities can be a really great tool, make sure to never use a silhouetted edge as what you are converting from. Converting from an edge is fine, but even that can lead to some unwanted changes depending on how your surface topography changes.

 

 

5) That cyan line you see on the screen means that it is an "open edge". With out being able to see the model, just know that there is a gap in the model and SW is trying to show you as such.

 

6) As far as that sweep not working, you have to composite the curves together into one path for the sweep. Again, sucks, but now that you know, life will be a lot easier.

 

7) 3D sketches tend to get "wonky" at times due to whatever solver SW is using behind the scene. If you are going to use it, try to keep in mind that the X,y,z system can trump some of the "traditional" relationships.

 

Here are a few sites that can more than triple the understanding of what SW is doing.

 

1) http://dezignstuff.com/blog. He also has a surfacing bible book that really explains all of the different surfacing tools and WHY they work and why they fail. When to use a surface fill vs a boundary surfaces.

 

2) Though some of the material is outdated, just due to what SW has added over the years, www.dimontegroup.com/Tutorials/SolidWorks_Tutorials.htm still has quite a few relevant tid bits. (i.e. WHY the shell tool fails and what can be done to avoid from doing that)

 

3) Two great sites with SW models to download....www.zxys.com/swparts and www.mikwjwilson.com. On the Zxys site, take a look at the "Auto Seat, Old School Fan, and Bootz" model. And check out the Mach 5 Speed Racer, sick surfacing model and that was in 2001 version of SW.

 

Hope this helps....

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