Why I can't split a solid model into 2 half using a spline for the cut?

Greetings:

I wish to split this part
http://home.comcast.net/~wangphk/SolidWorks/CutFailed1.jpg into two
different parts top and bottom and still reference to the original one
in case there is some design change. Unfortunately, I am unable to
use the spline curve to make the cut. Effectively, I receive a
message "Unable to make feature as specified" . However, I don't have
this problem using a straight line. Am I missing something?

Thanks in advance for your time and help.

 

I think you need to use the split tool not the cut extrude.

Corey

 

Your screen shot at the bottom shows the split parts. At the top you
are trying to do a cut, but you have used the split function to create
the parts at the bottom. I don't understand.

Anyway, first do a Tools, Check to make sure that the model is ok.
Assuming it's ok, then use the Face Curves function to see if you have
degenerate faces (where face curves converge to a point).

If you are converting the parting line, you might also want to try to
extend the spline past the borders of the part, or use the spline to
create a surface which you can extend, and then use the surface to cut
or split the part, whatever you are trying to do.

It may be that the converted PL at the end closest to the boss has a
funny little curl to it. You could test this by making the PL flat at
the ends.

You might also try converting (or making a derived sketch of) the sketch
you used to make the PL split line instead of converting edges.


matt


(John) wrote in @posting.google.com:

 

I've found that this is very important when working with tricky surfaces and
edges. Downstream features are much happier when you can work from the
sketches instead of converting model edges. Little errors seem to propagate
and grow, eventually blowing your model up. Kind of like a butterfly
flapping his wings resulting in a tornado ten thousand miles away. -

Jerry Steiger
Tripod Data Systems
"take the garbage out, dear"

 

John,
Try extending your spline out beyond the part on both ends, either buy
extending the actual spline or by adding tangent lines to your spline.
Let us (me) know how that works. I would be interested to know. It's worked
for me in the past when I couldn't get something to cut.

Muggs

 

Thank you all for your input and help.

Corey: I did use the split tool. However, I have two surfaces (top &
bottom) instead of two solids.

Matt:

<<Your screen shot at the bottom shows the split parts. At the top
you
are trying to do a cut, but you have used the split function to create
the parts at the bottom. I don't understand.>>

I thought the split parts will give me two solids; however it gives me
two surfaces instead.

<<Anyway, first do a Tools, Check to make sure that the model is ok.
Assuming it's ok, then use the Face Curves function to see if you have
degenerate faces (where face curves converge to a point).>>

I did a check for All, Solid, Surfaces, Invalid Surfaces, Invalid
edges. As a result I have 3 open surfaces (Split Line1, Parting
Line2, Parting surface1) with an arrow pointing to the same point. Is
this preventing me from cutting using spline?

<<If you are converting the parting line, you might also want to try
to
extend the spline past the borders of the part, or use the spline to
create a surface which you can extend, and then use the surface to cut
or split the part, whatever you are trying to do.>>

If I extend the convert parting line by deleting the constraint at
both end so I can stretch it freely. The spline shape is no longer
the same as the parting line.

<<It may be that the converted PL at the end closest to the boss has a
funny little curl to it. You could test this by making the PL flat at
the ends.>>

I don't get this. It seems that I don't have any option to make the
PL flat at the end. Do you mean I should sketch 3 segments, both ends
is a line and the middle section is pl?

<<You might also try converting (or making a derived sketch of) the
sketch
you used to make the PL split line instead of converting edges.>>

I try buy selecting the splitline sketch + ctrl + select front plane +
Insert + Derived sketch but I receive "sketch cannot be inserted using
the currently selected edge" message.

Jerry:

I re-sketch my spline, constraint its control points to be coincident
with the split line sketch point by point and it's working. I can now
cut the part into 1/2 top and bottom.

 

If you want solids instead of surfaces try adding an extrude thickness (or
knit and try to form solid) you can specify to create a solid from enclosed
boundry.

Corey

I think from your post script that you got the desired results, was that an
acceptable solution or do you prefer using the first sketch?

 

That's a bit scary. Splines are touchy little creatures and making sure that
they really match is not very easy. Just because the points are coincident
doesn't mean that the resulting splines will be the same. Since it sounds
like you have the original sketch to work with, it seems like you could just
share the sketch or convert edges from the original to the new sketch. Much
safer. Of course, you should have been able to use a derived sketch as well,
so there is something funny going on that I don't understand.

Jerry Steiger
Tripod Data Systems
"take the garbage out, dear"

 

Are you starting with a solid? There should be folders at the top of
the tree that show solid and surface bodies.

If you have solids and surfaces, it might be that when you selected what
to "split", you selected the surface bodies instead of the solid bodies.

The parts are named "Mold_Tutorial-Core Surface Bodies", so someone
knows that this is a surface.

Maybe. The error you mentioned might occur if you are cutting nothing.
You can't cut surfaces, you have to trim them (just a silly terminology
thing). If you don't have a solid to cut, then I could understand why
you would get that error.

That's not what I mean by "extending" the splines. You're changing the
size of a proportional spline when you do that. Along with what you
said to Jerry, it looks like you have to do some homework on working
with splines.

What I meant by "extending", is this: Draw a circle centered on the end
points of the spline, and use the Extend tool on the sketch toolbar or
sketch tools menu to extend the spline up to the circle. Try with a
small circle first.

I was just thinking that to troubleshoot what was going on, you could
make both ends of the PL horizontal. One side is already horizontal,
but the other side seems to end on a slant. PLs ending in a slant on a
curved part which are then projected onto a flat surface with convert
entities will often create a little curl at the end with a tight radius
that makes life miserable.

Well, the message seems to indicate that you have an edge selected. Try
selecting the sketch and the plane from the feature manager.

That's because the spline doesn't match your PL, and if you click on the
cut feature in the tree, you'll probably see that it highlights small
cut faces.

You might consider getting someone from your reseller to sit down and
work through some of these issues with you. There are some basic
concepts which you don't seem to understand yet. This part was part of
a tutorial? Where did it come from? Are you sure you've followed the
steps correctly? Did you get these with some book or some trial version
of a product you downloaded?


matt