yellow errors OK?

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
right.
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
persnickety???
jk
Reply to
John Kreutzberger
Loading thread data ...
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 mistakes.
Reply to
That70sTick
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 neurotic.
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.
Reply to
Seth Renigar
John,
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)
Mark
Reply to
MM
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.)
WT
Reply to
Wayne Tiffany
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.
Reply to
TOP
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 expensive.
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. Ed
Reply to
ed1701
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.
Bo
Reply to
Bo
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....
Scott
Reply to
IYM
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.
Thanks, everyone.
jk
Reply to
John Kreutzberger
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.
WT
Reply to
Wayne Tiffany
IYM,
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 John.
Reply to
TOP
Ed,
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.
Mark
Reply to
MM
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 bogus spots)
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.
Reply to
ed1701

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.