endpoint is wrongly shared by mulituple entities?
Paul Dewitt
The sketch cannot be used for a feature because and endpoint is wrongly
shared by multiple entities.
The system highlights green lines and after trying to analyze the endpoints
at the end of the 2 green lines I can't see any thing wrong.
Could someone tell me what the most common mistakes or way to find the
problem?
Thanks,
EvadeM
"Paul Dewitt" <dewi...@bellsouth.net> wrote in message
news:sm5P9.6946$a%4.1745...@newssvr10.news.prodigy.com...
aren't three lines sharing an endpoint?
Dave
Paul Dewitt
The system verifies which entities have a problem by turning them green
right? I only have 2 lines that meet that are green so I extended them then
trimmed them again to make sure there only 1 endpoint where they meet. Any
other ways to check them?
Paul
"EvadeM" <san.rr.com@dmerrifield> wrote in message
news:rD5P9.35002$B31.7...@twister.socal.rr.com...
Paul Dewitt
for duplicate entities? I though SW was smarter than to allow more than 1
entity to be in the same space.
Oh well, thanks for the help.
"EvadeM" <san.rr.com@dmerrifield> wrote in message
news:rD5P9.35002$B31.7...@twister.socal.rr.com...
>
matt
One way to test for that is delete one, see if there is still a line
underneath, if not, then ctrl-z (undo).
If you see any sketch lines on the screen that are visibly narrower than
the other lines (as narrow as dimension lines), that is another
indicator of that error.
Also, if you don't have Tools/Options/Sketch/Display entity points
turned on, then turn it on. It will help you find extra endpoints that
don't belong.
Sometimes you can drag a window around corners to see if there are very
short segments hanging out. SW will highlight any line that is inside
the dragged window.
matt.
EvadeM
> I found a duplicate entity that was the problem. Is there a way to check
> for duplicate entities? I though SW was smarter than to allow more than 1
> entity to be in the same space.
>
> Oh well, thanks for the help.
You can check your sketches with tools, sketch tools, check sketch for
feature. This would have given you the same message. To get rid of duplicate
entities use tools, sketch tools, repair sketch.
Dave
Jerry Forcier
Can you say more about the skinny sketch lines I sometimes see?
Sincerely,
Jerry Forcier
ms
Then using "Circular sketch and repeat" to make a pattern of 3 arcs about
the center point. (Think windmill). I then wanted to extrude thin features
of the arcs but get the error. Seems like a simple thing that Solidworks
should be able to handle. What I ended up doing was extrude one arc and then
make a circular pattern, but had to make a small diameter cylinder at the
centerpoint to prevent a disjoint body. Any ideas on how to do this without
making the cylinder at the center. I'm on Swx 2001+ SP6, scared to make the
jump to 2003 until SP1.
"Jerry Forcier" <jfor...@attbi.com> wrote in message
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EvadeM
"ms" <artisan_d...@attbi.com> wrote in message
news:hZgQ9.374242$pN3.42861@sccrnsc03...
> Is this a bug? I wanted to do something similar by drawing an arc segment.
> Then using "Circular sketch and repeat" to make a pattern of 3 arcs about
> the center point. (Think windmill). I then wanted to extrude thin features
> of the arcs but get the error. Seems like a simple thing that Solidworks
> should be able to handle. What I ended up doing was extrude one arc and
then
> make a circular pattern, but had to make a small diameter cylinder at the
> centerpoint to prevent a disjoint body. Any ideas on how to do this
without
> making the cylinder at the center. I'm on Swx 2001+ SP6, scared to make
the
> jump to 2003 until SP1.
>
Make your thin extrusion. Make your first sketch shown. Create a new sketch
and use convert entitiy on the construction arc. Make a thin extrusion.
Dave
matt
The skinny lines aren't a bug, they just tell you when you've created a
sketch that can't be used to create a feature. Whether it is a good
idea to have this limitation or not is a different argument, but the
skinny lines are intentional, and that is what they are there for.
Here's a little example. The rib feature can use a wide variety of
sketches that make other features puke. Say you draw an "L" then
another line not connected to the "L", for example, "L1". The rib
feature works with disjoint open or multiple open/closed contours, even
if you were to put an "O" on top of an "X"! (The "X" works if it is two
crossed lines or 3 lines with two of them colinear, but it will not work
if it is 4 lines that meet at a point). But if you connect the single
line at the vertex of the "L", the rib feature fails. I think this has
to do with how SW figures which direction the thickness goes, same for
thin features. If it is a string of lines end to end, the thickness can
be to one side or another, or both, but if you have 3 lines that meet at
a point, the only choice that makes much sense is the "both", even
though that doesn't work. It would be useful if SW allowed this, but
currently it does not. It seems inconsistant that a "T" or a 3 line "X"
rib will work, but a 4 line "X" will not.
Anyway, maybe this just rubs salt in the wound, or confuses the issue
more than necessary, but it is a valid request for surfaces, ribs and
thin features, but still not valid for sketches for solid features.
matt.
Jerry Forcier
Thanks much for responding (like you so frequently do).
Robin
end point. This often appears when you have two lines joined and a third
really small that you cannot see. Try to windows select the end point and
it will select the small line if there is one. There you can delete it.
--
Robin
Mech eng
SW2001 SP14 &SW2001+ SP5.1
AMD 1333 512 ram
Spaceball
Hacked GeForce 3 to Quadro
"Paul Dewitt" <dewi...@bellsouth.net> wrote in message
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