Newbie..extrude cut @ an angle ??

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.

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.