interpolate between two lines

[wwwworks]

Hello everyone!

I am struggling to create a body that is shown in the image.


I have 2 drawn two lines, blue and green. I'd like to interpolate between them and create a body without sharp corner.

The blue one is at 30degrees and I'd like to gradually bring it up to 90 deg so that is connects with the green one. The leftmost points of the green and blue lines are collinear. How would you create such body? I don't mind if we are cutting or adding material.

[matt]

One way to do it is to loft a surface between blue and green, split the surface blue is on with the blue sketch, then use Replace Face to replace the small faces next to blue and green. You might have to sketch guides between the ends of the blue and green to make it all fit nicely. An easier, sloppier, faster way of doing it would be to just put a big honking fillet on the edge between blue and green. You could try a fillet with hold lines, better yet a face fillet between the faces you ultimate want to connect (above green, below blue).

A third way, now that I think of it is to use Delete Face to get rid of the triangular face next to green, and then use a fillet on the edge between the resulting faces.

EDIT: I should add that what you are asking for will result in a zero radius corner. If you're machining this, you might think of another way that will give you something more easily machined.

[zxys001]

..yeah, Delete Face should work (image attached)

[wwwworks]

Thank you both for helping out. I tried the delete face and add fillet. Unfortunately the corner marked with blue dot is lost, because it also gets filleted.

This part will be machines on a 5 axis water jet. It is first one so there may be some problems, but from what I've seen on youtube, it should be possible:


The jet cutting head would start at 60deg angle relative to horizontal table (blue line) and straighten it self to perpendicular (green line) while maintaining the same vertical direction. Jet entry point is on the back side of images attached.

[wwwworks]

Ahh. I figured it out. sort of. The shape I am trying to draw has a name =>helix. This one has also been partially cut. This is the right shape and it interpolets between the two lines the same as a jet would. I'd like to make a solid body out of it. I draw a rectangle and made an extrude to helix surface, but solidworks rejected helix surface as viable extrusion end surface. Any ideas on how to use this helix as body surface?

[Dwight]

I tried the delete face and add fillet. Unfortunately the corner marked with blue dot is lost, because it also gets filleted.

You can save the cusp at the blue dot by adding a variable radius fillet and assigning the radius 0 at the blue dot end.

[Austin Schukar]

Would Face Fillet with Hold Line option work for you?

[zxys001]

Ahh. I figured it out. sort of. The shape I am trying to draw has a name =>helix. This one has also been partially cut. This is the right shape and it interpolets between the two lines the same as a jet would. I'd like to make a solid body out of it. I draw a rectangle and made an extrude to helix surface, but solidworks rejected helix surface as viable extrusion end surface. Any ideas on how to use this helix as body surface?

..yeh, you can also do split-lines normal-to and provide a spline (top/btm) profile to do a ~track of the jet... (image)

[Krzysztof Szpakowski]

The problem in your case is that the red point lies at the intersection of the green and yellow lines. Ergo - interpolation between red and purple points is a straight line segment.

So basically the surface you're "looking for" is a slice of a irregular cone with a vertex at the red point. For a better result, enter a small rounding in the red point.

Gretings

EDIT
Before adding the Loft, you can move the bottom surface aside to thicken the element, e.g. 0.5 mm. After making the "pass" you do the offset again to get back to the correct thickness. This way you will also get a small "rounding" on the bottom edge.

[Krzysztof Szpakowski]

..yeah, Delete Face should work (image attached)

Or cut with option Up to surface