not closed sketch

[david.johansson]

Hello


Sometimes when i have made a sketch that i will use later on it complains that the sketch isnt closed. Does someone know a good way to make the sketch closed in an easy way. Im tired of trying to zoom in and searching for the "gap"

 

[vlad1979]

[url]http://www.mcadcentral.com/proe/forum/forum_posts.asp?TID=34 294&PN=3[/url]

 

[david.johansson]

yes, in wf2

 

[[-Skint-]]

I use wildfire 3 and I still have this problem on numerous occasions when inserting and creating complicated sketches. Most of the time wildfire helps out by selecting the "broken" sketch with a red circle, however sometimes it doesnt show up and I too have to go through the sketch until I manually find and repair it. Its a true pain in the arse.. but something ive got used to and good at resolving

 

[AHA-D]

If you keep sketches simple - and thus keep features simple - and thus stick to robust modeling - you don't have much issues with sketches. I often wonder why people want to do an entire part in one go when it's only a question of making a base part, add a flange, create a cutout, throw some rounds in and mirror the lot about a symmetry plane.


My 2 eurocents ...


Alex


PS


...and you can do a lot without open (but aligned) sketches also (probably used to be a problem in early ProE).

 

[trillicomm]

There must be a config option that flags the Open lines/circles/entities in Different Color until they all become closed (contour). Make it real time. I bet SW already figures it out.

Keep the sketch as simple so that you don't need to zoom in too much to find the smallest gap.

 

[csusie]

WF4 has a resolve tool to help find problems with sketches such as gaps.

 

[[-Skint-]]

AHA-D , your exactly right and I agree. My problem is that I have to create very specific customer profile pieces which are very complicated shapes, in-order to mimic these shapes as best as possible I always import a dwg, dxf or .ai file etc, then my problems start............

Occasionally the whole complicated sketch will work first time, i think the problems originate from the cad files.

 

[david.johansson]

skint^^ i also have to do a very specific shape , AHA , i will keep in mind to do it so simple as possible but sometimes its not possible

 

[michaelpaul]

I bet SW already figures it out.

at least as far back as SW 2005 there was an option in sketch tools to check the sketch for a particular feature. for example, if you wanted to create an extrude, you would go to the sketch tools and select extrude as your feature type. the software would then verify that your sketch conformed to the requirements of an extrude (i.e. closed) and tell you there was a problem and show you where the problem was. I miss this..............

Michael

 

[SRINIVASANIYER1]

]


specific customer profile pieces which are very complicated shapes, in-order to mimic these shapes as best as possible I always import a dwg, dxf or .ai file etc, then my problems start

Open the dwg in autocad, convert to a JOINED POLYLINE. This would ensure that your parent data is TRUE.


Now import the dwg into proe.

 

[Jacoolo]

why do we mention SW when Pro\e is by default equiped in such a tool. You won`t find it in any menu. Just take it in mind - Pro\E will always check your sketch and shows you where and why it does not pass the requirment if you make it as internal sketch!

When You first make a sketched curve and than extrude from this - there is no tool to check this sketch. But if You first make an extrude and then make internal sketch Pro\e will always check it

 

[robrific]

I have imported from Acad and hadclosed sketch problems only to find that the Autocader had lines on top of each other.

VERY hard to find.

 

[SRINIVASANIYER1]

I have imported from Acad and hadclosed sketch problems only to find that the Autocader had lines on top of each other.

Exactly the reason why you should convert the profile into a pline in AutoCAd. Select the pline and put it on a unique layer. Then Tools>qselect> select all the components that does not lie on this unique layer. delete them.

 

[michaelpaul]

I have imported from Acad and hadclosed sketch problems only to find that the Autocader had lines on top of each other.

Exactly the reason why you should convert the profile into a pline in AutoCAd. Select the pline and put it on a unique layer. Then Tools>qselect> select all the components that does not lie on this unique layer. delete them.

does anybody else think it's asinine that we're recommending using another CAD package to get data into a form that Pro-E can understand and utilize?

Michael

 

[prohammy]

I have imported from Acad and hadclosed sketch problems only to find that the Autocader had lines on top of each other.

Exactly the reason why you should convert the profile into a pline in AutoCAd. Select the pline and put it on a unique layer. Then Tools>qselect> select all the components that does not lie on this unique layer. delete them.

does anybody else think it's asinine that we're recommending using another CAD package to get data into a form that Pro-E can understand and utilize?

Michael

michaelpaul,


Re your last comment, all we are talking about here is making sure that the data set (curve set) is in the form required for the design intent. If youwant to import a load of lines that are open, then you can do so. If you want to import a closed set of lines, then you can do that. The only point about converting the AutoCad line set to splines is that you know before you import that it is a closed set. The other alternative is to import a set of data and then use the trim tools to turn it into a closed set in ProE


Kev

 

[SRINIVASANIYER1]

Thanks Prohammy,


You drove home the point.


Dear Michaelpaul,


We should not shirk away from using any other software. After all Proe like Autocad is just a tool. The idea was to edit the data for import in the original software itself before taking it inside proe. This eliminates the mess that proe puts in in the form of dimensional constraints with the intent manager on.

 

[ctolman]

Well, if you are trying to keep everything ligit it is sometimes difficult to be using two different pieces of expensive software folks! That is my only drawback to throwing in AutoCAD as a tool.


I have had your problem several times. I have to create some complex geometry that has been imported for Aerodynamacist tools. The only hint I can give you is that using the trim tools to click almost every intersection in a complicated sketch is almost always faster than trying to zoom in on every intersection and find the error. If someone knows of the config operations that will keep a problem highlighted I would lo e o see it.

 

[SRINIVASANIYER1]

Use the AutoBildz route. It not only checks the profile but also highlights overlapping entities.

 

[Jacoolo]

and Autobildz is free, God bless PTC ))))