Wow, Walt first thanks for this helpful respons. Your ideas about reducing
the complexity to help Inventor find the extrudable areas sounds all more or
les reasonable. This will help me for sure. Although it doesn't give a
software-user much satisfaction how to save the software !!
Your quick workaround is an option (already done), but takes away the
efficiency and power of the master sketch.
By the way should it help to set the Contstraint Placement Priority to
Horizontal/Vertical ? I will test this.
Overall there's still no explanation for the difference in finding
extrudable areas between derived parts and masters.
Regards, Willy
"Walt Jaquith" wrote in message
news:BC94C78F2FF0418DDA1B8DB501A34C25@in.WebX.maYIadrTaRb...
> Hi Willy,
>
> One of the drawbacks of a single sketch that has multiple extrusions is
that
> Inventor has to 'find' all the possible extrudable areas, and this can
take
> a while. I use master sketches with many possible extrusions, and have
seen
> the problems you're describing. I have turned in a few cases where
Inventor
> couldn't find the extrudable area in the derived part when it could find
it
> with no problems in the master. Some of it has to do with the sheer
> complexity of a master sketch. We are doing things with Inventor that are
> beyond what the designers envisioned.
>
> There is something you can do that may help both your problems. I've
> noticed that it apparently matters to Inventor just how a shape is drawn.
> If you are drawing a polygon, and start at a certain point, then proceed
> through a series of points, and finally click back where you began to
close
> the profile, Inventor will have no trouble finding that area to extrude.
If
> you draw the same polygon in parts, starting and stopping the line
command,
> Inventor still does ok. But draw one of those line segments backwards in
> relation to the others, and you just might have problems when you get that
> profile into a derived part. I've never seen this happen when there was
> only one profile in the sketch, but get 20 possible profiles in the same
> sketch, and things can get a bit rough. I have had cases where I deleted
a
> line and redrew it in the opposite direction from the original, and
suddenly
> the area was extrudable. A slightly different constraint scheme for that
> profile can also cause it to suddenly start working. It's possible in a
> master sketch to have several lines coming together at a single point.
> Example:
>
> ________
> | |
> | |B
> |_______|___C___
> A | |
> |_______|
>
> The two extrudable rectangles meet at their corner. If the endpoint of
line
> A is actually constrained to the endpoint of line C instead of line B,
> Inventor seems to have to work harder to compute the upper left rectangle.
> Are the endpoints constrained together in a way that makes it easy for
> Inventor to find the extrusions? Theoretically it shouldn't matter, but
the
> fact remains that I see far fewer profiles fail to extrude, and my
> extrusions compute much faster since I started paying particular attention
> to how I constructed my sketch profiles.
>
> Another thing I've noticed: If you draw a rectangle, and either
right-angle
> or parallel constrain the lines together (normally, Inventor does this
> automatically), then add dimensions between the lines to define the size
of
> the rectangle, there is actually a sort of overconstrained condition going
> on. Inventor allows it, but putting a dimension between two lines is kind
> of the same thing as saying that they're parallel, right? Normally this
is
> no problem, but when you push the envelope with a master sketch setup, it
> can become an issue. Another weird asci example:
>
> a ____W______b
> | |
> X| |Y
> | |
> |___________|
> c Z d
>
> If you already have parallel or right-angle constraints between lines
W,X,Y
> and Z, and then you put a dimension between lines X and Y, you've actually
> slightly overconstrained the sketch. For a simple rectangle like this,
it's
> not a problem, but in a complex master sketch I've seen it cause issues.
> The answer is to place the dimension between line Y and point a instead.
It
> does the same thing without causing a potential glitch.
>
> If you already have a complex master sketch that you're having problems
> with, there is a quick workaround that can help. In the derived part,
edit
> the sketch you're having trouble with. You won't be able to change any of
> the existing lines, since they're all linked to the master, but you can
add
> lines. If an extrusion isn't solving, trace it's outline with a new set
of
> lines. The lines you add will constrain themselves to the existing line,
> and the profile should solve. Any changes made to the master sketch will
> update the lines you added, so adaptability isn't lost.
>
> Cheers,
> Walt
>
>
> "Willy Driessen" wrote in message
> news:ABC227AB6B966AEDFAE22FA7293A6383@in.WebX.maYIadrTaRb...
> > I'm trying to use a master sketch which comes with a derived part for
> extrusion.
> > This (derived) sketch containts about 50 lines, all fully contstraint.
The
> sketch forms several "extrudable" area's.
> > Starting the extrude command let's me wait 19 seconds before the sketch
> appears again.
> >
> > Question:
> > 1. how to reduce this waiting time (settings ?)
> > 2. some area's are not to select (the + sign not to show them),
although
> in the derived part itself they are.
> >
> > Any suggestions ?
> >
> >
> > W. Driessen
> >
> > System:
> > Dell Workstation 350
> > 2.4 GHz
> > 1 Gb Ram
> > Quattro 750 XGL
> >
>
>
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