Newbie..extrude cut @ an angle ??

Need some guidance here......
I am going brain dead or am totally missing something. I think this is a
direct result of working with ACAD toooo long. :<) Am playing with SW2004
to get a sketched shape (viewed from the front)to extrude cut thru a
rectangular block (viewed from the side)@ 14 Deg going down from left to
right. I can make & position the sketch fine on the face of the block...but
I can't figure out how to make it cut @ the 14 Deg. angle. Why can't I boss
extrude the sketch...go to the side view...rotate the extrusion 14 Deg and
subtract (cut).? Or am I making this too complicated ?

Thanks
Gene

 

Yes, from the sounds of it, you ARE making this more complicated than
need be. It is difficult to make out what you are trying to do. Seems
to me, you are trying to apply Acad methodology to SWX (a common hurdle
among new users).

Suggestion #1:
Read the Getting Started and On-line Tutorial (Look in the Help menu).
YES!!! READ THEM!!! It will help you out.
Also, SWX just released a SWX 2004 Reference Guide, a comprehensive
manual for SolidWorks, in PDF format. You can get it at solidworks.com
in the subscription support section.

Suggestions #2:
If I understand you correctly, you could sketch a new line on the side
of your cube pointing in the desired cut direction, then in the
direction box, select that line when making the extruded cut. (This is
a new feature of 2004, I think)

Suggestion #3:
Create planes so that the sketch normal is pointing in the direction you
wish.

Hope this helps, Good luck.

 

Gene,

I sent you an email, but here is what I think you want...?

Draw your solid rectangle box. On the front face, draw a sketch of your cut
(Sketch2).

On the right-side of the block, draw another sketch (Sketch3) with
construction lines, one of them going down and to the right at 14deg, and
the left end point tied to something in Sketch2. Rotate the model if
necessary to see both sketches at once.

Now highlight sketch2 in the feature tree, click on Extrude_Cut, and in the
second empty selection box (Tool tip of "Direction of Extrussion"), pick the
14 deg angled line from Sketch3. Set the other stuff to whatever, blind,
through all, etc.

Click the checkmark, and you should have what you want, unless you wanted
something that I didn't understand....?

Mr. Pickles

 

Thanks for the response,
I only have one question, because the sketch is vert on the front face and
you are extruding it @ 14 Deg relative to the vert plane wouldn't it create
an elliptical cut ?? Wouldn't I need to rotate the sketch to 14 Deg to
achieve a true circular cut ??

 

Yes, this method will produce an elliptical cut. I will send you an
example of one way this can be done.

The key is to somehow create your sketch plane at the 14 deg angle and
THEN extrude the cut.

 

OK
I am definitely doing some serious reading...but...these answers just bring
more questions I need to research.
1. I guess I can't rotate the sketch to the 14 Deg.! (too simple, why ?)
2. Can I create a construction plane using the (extrusion) sketch as the
points for construction.? (yes)
3. Then can I rotate the plane with the sketch on it.? (not sure)
4. Do I need to "re"construct the sketch "on" a rotated plane. (need to
construct angled plane)
5. I will need to move the sketch & plane to a point in space where it will
create the cut in the proper place on the base block.?

questions...questions...questions...questions... ;-)

Thanks

 

OK, I sent you an example file of what I think you are trying to do.
Hopefully, it helps. Let me know if you do not get it.

I think you are on the right track when you mention creating a
construction plane at your desired angle first and then sketching your
cut profile on that.

Unlike Acad, the ORDER in which you do things is VERY important in SWX.
With Acad, only the end result really matters. But, with history based,
parametric modelers like SWX, the method of getting there is equally
important.

 

1. I guess I can't rotate the sketch to the 14 Deg.! (too simple, why ?)
Rotating it 14° is possible, but it will take a little definition. Why?
Well, 14° in reference to what? There are an infinite number of axes that
it could be rotated around - the software could pcik one automatically for
you, but it would be wrong almost all the time.

The easist way is to draw a sketch line that defines your direction vector,
then click the line and its endpoint and create a plane normal to curve,
assuming that the new plane ought to be perpendicluar to one of the default
planes. If that assumption is off, draw a sketch line on the current plane
you are on, then use that as the axis for folding off the 14° plane you want
to create.

Once a sketch is on a plane, it will always rotate with that plane. You are
now in a parametric world - child features (your sketch) are defined by
their parents (the plane). Change the parent, and the kid changes too.

Nope. No reconstruction required This is also part of the 'parametric' bit.
You can RMB click the sketch at any time and edit the plane it is on - from
the current to the new, rotated plane. You just need to be sure that the
new plane is at the right place in history so it can become a parent for the
sketch. Think of the feature tree as a family tree - the grandparents have
to come before the parents, and both have to to come before the kids.

Once on the correct plane, you should be able to use sketch references to
place the sketch in the correct position.

It is very wierd at first, but it will all make terrific sense when you get
the hang of it. After I got it, I couldn't fathom working any other way.