just wondering how others feel about this.
For my work, I don't allow any sort of error to exist in my models; red or
yellow. If a sketch entity is dangling-I fix it and move on.
Right now I am working on a project of injection molded parts. They are all
coming in with at least 3 of those yellow error warnings on the feature
trees. Every time I get another revision, I need to fix all of these just
for my peace of mind. The designer says they are not errors and won't
address the issue. Maybe he has bigger problems, but to my it just isn't
At SWW I was in a session given by a SW employee that I respect. One of the
models in his presentation had some of these errors on them. Another person
in the session questioned this, and he just said that these are OK.
To me this is at best lazy modeling-anybody want to tell me I am being too
I don't allow them, either. No reason not to fix. Leaving them yellow
sends one of two messages:
1.) There is a real problem that needs to be fixed.
2.) Guy who left them is liable to not correct other more important
To reinforce your feelings, I don't think you are not being to persnickety.
Maybe a little neurotic however.... :-) But that's ok. I'm just as
Seriously though, I agree that it is simply being lazy. If there is a
problem, FIX IT. These errors ARE problems. That is the whole point behind
having an error in the first place, to let you know that there IS a problem.
With that being said, there is also the chance that simply ignoring these
errors from the product designer won't effect your end of the job either.
So, it may be a toss-up whether to fix them or not. You will have to be the
judge of that.
It "is" just lazy ASSED modeling,,period. I think the SW guy meant that they
were OK (for now) inasmuch as they weren't relevant to what he was doing
(demonstrating) at the time. If he really believes that (and worse yet
teaches it), he should be fired.
Sounds like your having to deal with a certain type of industrial designer.
Any ME who believes that either needs to retire, or has no clue as to how
the software really works.
Whenever I get something like that from anyone here, I make them fix it. I
also make sure I know exactly what the problem is before I send it back, so
they can't cheat. It doesn't happen that much anymore.
Of course, if your a vendor supplying a service using customer data, ya just
gotta bite the bullet and fix it yourself (I guess)
They are not errors??? What are they - hood ornaments? Curtains?? Errors
are errors and little errors can grow into bigger errors. Every time SW
hits something it doesn't like, it tries to resolve it, and after trying and
failing, it flags it. Sooooo, read that as lost time. If your issue is
in-house, pin him down as to when he WILL fix the errors. If they really
are insignificant, ask him to suppress the things (parts/features) causing
the errors. If he says, well, those things are needed, then tell him that
they then deserve to be correct, not just getting by - fix them! Stupid,
lazy people! (My opinion, suit on.)
SW has typically had two problems with errors. The first is not
flagging them when they exist and the second is flagging them when they
don't. The first type can be most aggravating. What does what's wrong
say about these errors? Does verification on rebuild or TOOLS/CHECK
with the feature option checked give any insight? Does CTRL-Q make them
go away? Remember errors can have errors too.
Usually they indicate 'dangling' errors, and though not a big deal from
a geometry creation standpoint they CAN be a significant problem from a
design standpoint - the model is no longer behaving as it was defined.
The person who made the relaitonships in the first place needs to go
back and check that the missing relationships aren't significant to the
model, and to indicate that HE/SHE is OK with the model by deleting or
reparing them. To aks you to guess is out of line and potentially
However, (there is always a however with SWx, isn't there?) there are a
couple of yellow errors that literally are nothing and you can't often
repair. The one that comes to mind is Shell - SWx will create a valid
shell by loosening its internal tolerances a little, and let you know
by adding a yellow warning. The model is fine (of course, always check
by doing a round trip import/export) and it could take a long time to
change to get rid of that yellow error (and you would have to guess -
when you get the yellow warning you do not get shell diagnostics)
There is another yellow error like that, but I can't remember what
feature it shows up on right now. However, the Designer should flag
those with a comment in the feature tree - the person designing the
part is repsonisble for insuring the mdoel is OK and communicating that
to anyone downstream.
I see the same thing when I design my plastic parts. Typically, I add
a radius or remove it and the plane it mates with gets a different
"edge" which is referenced in a sketch somewhere down the tree.
I absolutely will not release a solid to a toolmaker without fully
constrained sketches without errors. It is just asking for trouble
later on if I don't fix them.
I agree with pretty much everyone else on this issue...Errors are errors.
I'll never release something with yellows (on purpose anyway). What I mean
by that is that when they typically happen to me they are almost 99% related
somehow to configurations. (i.e., in one configuration it's fine, but you
change to another and you have yellows popping up) and most of the time they
are mate issues. So I'll make a modification and everything will look fine,
but sometimes I'll forget to check all configurations to make sure none have
a problem with the change. Is there a way to have Solidworks automatically
check all configurations for errors without me having to go through each
one? Just curious....
I appreciate all of the comments. I wanted to see how many responses I got
before jumping in again.
The errors that have been bugging me are definitely due to dangling sketch
entities as Ed (and others) suggested. At my insistance the designer finally
cleaned them up, with interesting results. He had been claiming all along
that these were dangling due to inadvertant realtionships that SW adds
during sketching and that he didn't have time to track them down. He was
pretty pissed off when the mold-maker told him that his delivery was going
to go on-hold until we got clean models.
Well, we got models today with clean feature trees and the parts had a
couple of significant changes. When he fixed the sketches (these were at the
very beginning of the FT) other interesting things happened down the tree
which resulted in new geometry. I feel vindicated. Guess this means I'll
continue being a PITA-good to have an excuse anyway.
Guess we all agree that with a very few exceptions, if you have errors at
the end, you didn't finish the job. It's nice to once in a while win one
for the good guys! Thanks for getting back to us on this.
As Ed pointed out, the shell errors are unavoidable and the yellow
placarding is just a warning. There is nothing you can do other than
delete the shell feature. But this doesn't look like what was bugging
You can usually see shell errors by using curvature plots or zebra stripes.
There will be noticable weirdness in the affected area. I've found that alot
of times its caused by bad tangency condition in the geometry used to define
the base shape, especially if splines are used. There are tools for
correcting these since at least SW2005.
Having a surface anomoly on the inside (core), or anywhere for that matter,
can really mess with the surfacing algorithims in a CAM program. Solidworks
"will" allow these types of errors to exsist even "without" a yellow flag.
Good tip on the curvature - I haven't tried that before.
I've also noticed I can see junky faces that were made in regualr
shading (if they are really obvious). The issue I have is that it is
not always obvious, though I will try to see if the subtle ones show in
curvature display. Shell diagnostics can be nice because you can see
the trouble faces that contribute to the shell problem - otherwise its
a guess (start cutting and shelling the model again to isolate the
The CAM program issue is also a potentially good point, but I have no
experience with what will work and what won't. After a roundtrip
import/export to confirm the model is stable I don't have the
background to say 'X will freak out CAM'. I have better luck fixing
bad spots after they are made (cut out the bad face and make a new one
in its place) than preventing them from being made in the first place -
its also a ton faster. So I might have a beautiful solid, but it will
still have that lousy yellow icon on the shell because my repair is
after the shell feature.