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

Greetings:

I wish to split this part

formatting link
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.

Reply to
John
Loading thread data ...

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

Corey

Reply to
Corey Scheich

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

snipped-for-privacy@yahoo.com.sg (John) wrote in news:559f7fc3.0404261008.c90b080 @posting.google.com:

Reply to
matt

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"

Reply to
Jerry Steiger

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

Reply to
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:

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 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.

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?

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.

Reply to
John

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?

Reply to
Corey Scheich

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"

Reply to
Jerry Steiger

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

Reply to
matt

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.