I'd like to remove the edges between the two faces in the picture thus creating one seamless, tangent, curved face:
Is there a tool or feature that is specifically used for this? I thought I might be able to use the delete and patch tool but it fails "due to geometric conditions". I've tried quite a few different things with no luck. Any help is greatly appreciated!
Go to Tools - Options and under Display/Selection check where shown in the red box in the pic below.
Hope this helps.
My guess is that it won't work because it looks like there are two separate features there.
Chris
Thanks for the help Christopher Estelow! I actually tried this shortly after I posted this question, but these are two separate features and the lines are still visible after turning off tangent edge display. Here's a pic from the top if it helps, as well as the part file.
You posted the model while I was typing the response above. And yes, the fillet tool will work. This one is 1mm. You may want larger.
Thanks for the help Glenn Schroeder! I tried the fillet tool but wasn't happy with the outcome due to the model still having the small indention where the two features (hook & lid) meet. I'm wanting them to have a continual surface with no geometry between them.
Do you mean this edge?
That can be fixed with a second fillet.
No, I'm talking about the edges reference in the image in my original post... I need the faces that create those edges to be a single, smooth face.
If the surfaces are tangent then Chris' suggestion should fix the problem. If not, you can try the fillet tool. That's typically what I do in that situation.
This is where I'm getting stuck... when I go back and make the sketch that creates the hook tangent with the circle of the lid I get all kinds of errors and the hook feature won't build because of it.
This one has trouble written all over it.
What you want is to design the handle surfaces such that they are already tangent. This does not want to play nice and merge with the original piece.
They hard way that works 101% of the time is to divide the solid faces where the tangent surfaces meet. Then, delete faces with the Delete Faces feature, turning the solid into a surface. Knit the handle surfaces to the cover surfaces and turn back into a solid.
Roland Schwarz, are you referring to using the split line tool to divide the faces where my hard edge is?
Yes. Sometimes just adding a split line is enough to get difficult parts to combine (e.g. tangent meeting edges). Otherwise... continue on with the hard hard way.
You could add a fillet at that edge right after the Body-Delete1 but before Fillet24. The two surface still won't be perfectly tangent but the transitions will at least be smooth.
If you make the radius very large like 200 mm then you will not have the obvious indent you mentioned before.
Hey Jamil Snead, that looks exactly like what I'm after. I can't notice the indent at all, however, when I try to create the fillet at 200mm on the same edges you have select in the previous picture, it says "Failed to create fillet"... I think it's because of my version of Solidworks (2011). What version are you on and could you possible attach the part with the large fillet you created, so that I can inspect it?
I am on SW2014. To get it to work I had to add the new fillet after the Body-Delete1 but before Fillet24. You won't be able to open my sldprt part but let me know if you want a parasolid just to see how it looks.
Jamil Snead, I tried your last suggestion and it worked perfectly! Thank you for the help!
