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Geometry Check is a tool inside pro\E which chceck the existing geometry if it contains errors.
That question is : what the errors are?
Some of them are just copy of list of errors included in german automotive norm - VDA 4955(as far as I remember)
So those are all things which could exist in geometry and cause big problems in :
*FEM analisys
*manufactring
*data exchange
some most unwanted ones are:
*manifold geom
*surfaces intersecting each other
*the surf is very close to but not touching
*and a lot of more which I do not remember
So in real Geom Chceck is not able to solve any problem, it is only an info. You personaly have to deal with them by changing the dim of features that cause a problem
What are common ways to deal with geom checks? Read this:
*change the sequence of feature
*try to be carefull with using edges as ref in sketches
*try to change dims to avoid problematic elements like - short edges
*divide big sketchers into smaller ones, it will help You to play with right sequence
*generaly, if it is possible - try to divide your model tree on first all features that creates external geom, second all feats that creates inner geom
*and in addition try to first add a material, than make a cuts
*and in the end - set up absolute geom
uff... I think this kind of info should spot a little light on this topic
everything you said is fine but the problem i am facing is: my models do not sho any geom check till i add drafts and rounds. the moment i start putting drafts and rounds. the error ocurs. anyway out for this?
so first type what kind of geom check You have - I can not read in others minds yet))
but I supposed You have - short edges, surf is close to but not touching?
so then, it is sad, but You only can change the dim for draft or round, or change the rounds to quilt and built them with merging with other surf then solidify
You can also put some drafts directly to sketchers - specialy for revolved surf
many ways - but remmember - if You already creates the geometry form 2d existing drawing, everything is possble with pencil and line, but not in ProE.
everything you said is fine but the problem i am facing is: my models do not sho any geom check till i add drafts and rounds. the moment i start putting drafts and rounds. the error ocurs. anyway out for this?
so it is better to start with the absolute. This kind of accuracy can make regeneration faster and could also help manufactring and DMU creation in assembly
I wonder which is the exact definition of Geometry Check.
It's possible to know some examples when this kind of problem comes out ?
It's depend on accuracy ?
How to manage these problems?
Are dangerous problems ?
For sure Geom Check could be dengerous, but it does not mean they mus to!
So the main unwanted geom check with solids are manifold problems, surf intersect each other, gaps and cavities.
It depend on accuracy - a lot. Some geom check are just tiny elements which YOu create without knowing about that. So usually they appear while cutting opertations.
Some of ways to solve this problem You can find in the previous topics.
But I can bet You want to have more detailed
Maybe - I say maybe - I will try to create a model with geomcheck and then show how to solve them. But I am not an expert of this kind of stuff. So all it would be just my experience
actually whenever ur geometery makesthe mathamatics of curves and surfaces ambigiuos, pro shows error msgs and complete the feature. this kind of errors should be checked by info geometry check. Its like a surface or curve lost one of its portion due to draft or any other cut or round. Actualy now-a-days its so easy to make rounds. But upto Rel 20, the people says that "if a person is expert of rounds, he is expert of pro with no doubts". some times we make gemotries that can not fullfill math, but we makes copies from manaully produced parts so we face the problems. But If we understand exactly, we can overcome it by changing dims by some microns. I will post an example soon.
I am starting a new thread, "shell challange". Plz check the part, and make it shell with 2.3mm thickness. Its going to be failed, pin point the problem and solve it and tell us all. ( I actually did it, but for your information and practice, I put it here). Try hard every one.
View attachment 3433
as You can see Pro\e highlight the sketch and place when the problem occur. In this case - sketch contains an element which is very close to existing edge. The change of sketch is necessary
2) This feature creates a tiny edge. The edge is highlighted on screen.
this case is a result of previous one. The elemnt in sketch cuts the existing edge and this cut is less or near the choosen accuracy. Solve first, this one will be solved automaticaly
3) The boundary of the highlighted surfaces was
extended. Unexpected results are possible. Try to modify the feature so that
extending is not necessary
in this case geom check is a result of merge feat. It happen that two surfs do not intersect entirely and pro\e has to make some new edges by its own. Solution - change the surf to intersect correctly or leave ti. It is not so bad geom check
4) The system could not construct the intersection of the
part and feature.
in this case the surf for cut was made first. Then Solidify func was choosen and cut was done. But, the problem is the the surf is larger then required and intersect with another solids surfs. Pro\e made a cut as reqiured but it recognize also the intersecting problem with another surf. Change the orig cut surf
cause of problem? - surf cuts another surf but not in whole lenght, in this case it is worth to make the solidify before round(if it exist), or change the cutting surf by extend func to not come close to another surf
in this case it is just example what could happen with rounds(one of many problems which could happen btw)
in general this can be solved by adding rounds with the same value at the front and at the bottom,
but lets imagine it is not allowed, so usually the best of the easiest ways to solve problems with drafts and round is right sequence - change the sequence of drafts and rounds and you will see how edge chain is changing. Badedge chain is main cause of round problem.
So we can assume that in this particular example changing the sequence is not enough either
Well, then, this can be done by using surfaces. This is how it could be done- make rib by surfaces, merge it, and create required round
I run into a lot of geometry checks in pro mold using imported parts for the reference model. In my experience if everything splits like it should and you get extracts then the geometry checks can be ignored.
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