Cutting a complex shape into a solid help

Hi everyone. I'm having a problem trying to cut a cone like shape into a solid.

I made a 3d sketch for the profile I wanted and then tried a number of tools but could not get it to cut properly. What would be the best tool for this? It's going straight to a point at the bottom of the solid so a loft wouldn't do it?

I also tried making a loft and positioned it on the corner but that didn't work either..

If anyone can help I would much appreciate it. I attached the file I'm having problems with.

CUTSHAPE.SLDPRT

Im not at a comp right now but you can loft to a sketch point. Ill try to open the file soon.

volume3K

What version of Solidworks is your file cutshape.sldprt was used to create the file?

Chubarka

Sorry, I saw the version after I asked the question. I am unable to open it with 2013.

Hi everyone. I'm having a problem trying to cut a cone like shape into a solid.

 

I made a 3d sketch for the profile I wanted and then tried a number of tools but could not get it to cut properly. What would be the best tool for this? It's going straight to a point at the bottom of the solid so a loft wouldn't do it?

 

I also tried making a loft and positioned it on the corner but that didn't work either..

 

If anyone can help I would much appreciate it. I attached the file I'm having problems with.

 

 

 

Here you go. I didn't spend time fixing any sketches but i would suggest that you use a 2d sketch for your Loft profile. The next thing i did was make a sketch point as the second loft profile. Is this what you are trying to do?

 

CUTSHAPE.SLDPRT

Thanks that looks like more of what I'm after! I'll go with that approach then. Appreciate it.

No problem. if you get hung up just post back. How do you plan on cutting that in reality?

It's going to be a mold from fiberglass in reality.

I'm still having problems. I've got a more final version of the shape I want but when I use loft it's too jagged.

Surface boundary seems to be the way to go for the right curves but it projects outside my original solid.

Here is the updated part I'm trying to cut https://drive.google.com/open?id=0BwDai0Z1ShR9cHJJcF81bzhYVTg

http://carsonimages.imgur.com/all/ The highlighted part of the pic are the planes I'm trying to keep straight without being cut.

Would multiple surfaces need to be used here? Any ideas?

One thing, which you may know, is that sharp corners in a Fiberglass mold are usually areas that bubbles/pockets form.

The image link isn't public so i can't see it.

One thing that happens from time to time is the graphical representation of the part isn't high enough quality(for PC performance). Go to your system options, on the Document Settings tab and down to "image quality". the first slider will increase the resolution of curves. See if that helps.

Loft and boundary should produce the same surface but there are some subtle differences. Make that image public and i will take a look.

Here is the image, I'll try those document settings when I'm back home.

Ideally I'd like to maybe draw it with 4 sides, one of the sides being the cone that cuts through to the bottom at a point. So many errors whenever I try to get this shape!

I was planning on Filleting the edges afterwards but maybe I'm better off trying to get the entire shape in one go?

I haven't had a chance to open the file yet but did the setti gs change anything?

Yes thanks I seem to have the shape a bit better to what I want. I'm still getting loft lines that I'd like to get rid of where the curves transition. I tried filleting but its still leaving black lines. I also looked in settings for tangent lines but couldn't see anything to turn them off?

I opened the file and im not sure what is going on. The loft cut isn't complete in the file.

Some general hints for you going back to the start of the file. You want to make fully defined sketches. When you have blue sketch entities that means they aren't fully defined(free to move). Unless you have a good reason(mine is usually with splines) you want to lock those down with dimensions and relations.

Next, lofts and boundary surfaces generally work better when they are going to the same number of entities. Example would be sketch S0 to S1. S0 is 6 sketch lines. S1 is 7. There are two lines on the top edge that could be one line. Solidworks ends up splitting faces and doing weird things in the background trying to figure out these patches.

Next, don't force too much to happen. I wouldn't build this hull in one lofted solid. i would work on one surface at a time. The bottom edge first. I have done a few hulls and reverse engineered some for customers showing them how to model them in Solidworks and this has always been my approach. Use symmetry(which you did) and work on a face at a time. Because you are working on big sections and small sections in a single feature you end up with some bad geometry.

Sorry i don't have any publicly available boat hull design videos. The best thing i have was a quick test i did awhile back that you can look at. Its not complex, and not complete, but it might help.

Boat Test.SLDPRT

Thanks that's been very helpful, I'll clean up the lines to start with. If I'm building it via separate surfaces and then cut into it with a cone, would it not be hollow inside and just leave me with a gap where the cut should be?

I presume I stitch the sides together once I'm done?

Thanks that's been very helpful, I'll clean up the lines to start with. If I'm building it via separate surfaces and then cut into it with a cone, would it not be hollow inside and just leave me with a gap where the cut should be?

I presume I stitch the sides together once I'm done?

If you knit a set of surfaces together that form a closed "water tight" region you can make it a solid