Problems using dwg file as a base part rel 2001

I have a 2D dwg file of some parts I have to model in 3D. I thought it would
be simple to go into sketcher, then select Sketch/From File, import the
lines I want, then use them as ref edges for the protrusions/cuts. Its
basically a flat plate with a complex profile, with about fifteen triangular
shaped cuts with filleted corners in it.
The problem I have is the whole section has over 100 imported lines/arcs. As
soon as I position the dwg in sketcher, Proe wants to calculate all the
dimensions (this also happens even with Intent Manager off, except a little
later on in the process). Then my computer hangs for a long time - perhaps
an hour or more. The processor is running at 100%, ram at about 50%. My
processor is 1.7Ghz.
I have resorted to importing small portions of the section at a time to get
around this (about 20 lines/arcs), but it takes ages to build up what should
be simple parts this way, and if you don't select one or two extreme
features with each import, the drag point for the sketch isnt in the centre
of the section so is difficult to place.
I want to be able to import the entire section and create a single
protrusion feature, then import the entire seciton of cuts and create a
single cut feature.
Has anyone got any better suggestions?
Is there any way to import the features in such a way that Proe doesn't have
to recalculate every single vertex?
Why is sketcher so cpu intensive?
Reply to
dakeb
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: I have a 2D dwg file of some parts I have to model in 3D. I thought it would : be simple to go into sketcher, then select Sketch/From File, import the : lines I want, then use them as ref edges for the protrusions/cuts. Its : basically a flat plate with a complex profile, with about fifteen triangular : shaped cuts with filleted corners in it.
Check this out from the PTC.com website. It's a free download, seems like something you could use. : : The problem I have is the whole section has over 100 imported lines/arcs. As : soon as I position the dwg in sketcher, Proe wants to calculate all the : dimensions (this also happens even with Intent Manager off, except a little : later on in the process). Then my computer hangs for a long time - perhaps : an hour or more. The processor is running at 100%, ram at about 50%. My : processor is 1.7Ghz. : : I have resorted to importing small portions of the section at a time to get : around this (about 20 lines/arcs), but it takes ages to build up what should : be simple parts this way, and if you don't select one or two extreme : features with each import, the drag point for the sketch isnt in the centre : of the section so is difficult to place. : : I want to be able to import the entire section and create a single : protrusion feature, then import the entire seciton of cuts and create a : single cut feature. : Have you tried using 'File>Open', selecting the type of file (SEC DWG DXF) and opening it directly? Using this as a 'template' for 'use edge' sections in sketcher might work. It won't be parametric, obviously, but doesn't sound like you need anything eleborate.
: Has anyone got any better suggestions? : : Is there any way to import the features in such a way that Proe doesn't have : to recalculate every single vertex? : : Why is sketcher so cpu intensive? : I run into this question a lot, seems to have it roots in the impression people have of sketching based on experience with drafting programs. The difference is parametrics and associativity. 2D sketching is basically connect the dots for creating draft entities. Until the last couple revs of AutoCAD, there was no connection between these entities nor between the entity and a dimension and, so, not really very much to keep track of. Pro/e, on the other hand, is using sketcher to create fully dimensioned, fully contrained geometry referencing other features. And every time you change something or create a new sketcher entitiy, it needs to calculate not only where it is, how it's constrained but what effect it has or what effect other geometry has on it. On top of all this, it is even checking the viability or integrity of the geometry for creating a solid. It warns of extra entities, it won't try to create a solid from an open section and warns you and it is even evaluating the geometry in terms of proportions, warning, for example, of short sides. So, I guess the short answer to that question is that Pro/e is just doing a whole hell of a lot with even a 'simple' sketch.
David Janes
Reply to
David Janes
I've never seen a variational solver that's not pretty quickly overwhelmed by things like that. Don't know if there's a way to turn it off (?).
Haven't been thru a similar experience, so don't know if it will help, but I think I'd try .....
_ Converting the polyline curves to splines, if possible (assuming you don't need hundreds of planar faces on the part).
_
Translating via IGES instead of importing the stuff into sketcher. It will still slog along quite a bit (if you are still using the pline curves) when you project the curves to sketch, but it's probably not as bad as importing into sketcher.
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Reply to
Jeff Howard
I don't have Acad and have no control how the files are created. I might try importing the dwg and exporting from Proe into IGES.
Reply to
dakeb
Importing the dwg and exporting from Proe into IGES, then using the iges file as the base part actually worked, much faster than importing into sketcher. Thanks for the tip!
Reply to
dakeb

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