Rounded Rectangle with 2 Radii

sam_biddle

I'm trying to create a rectangular shape with 2 different radii that transition smoothly together.  I'm having trouble recreating the drawing from a blueprint without having a noticeable break between the different arcs.  I created 4 arcs of one radius and 4 of another, but they don't join well together.  Does anyone have an idea about how to best do this?  I have included by sketch document along with the blueprint drawing that I'm working from.  I'm grateful for any help.  Thank you.  

This is what I'm trying to reproduce:

Here is a link to my document: https://cad.onshape.com/documents/2c34f733174440224b37246d/w/a0faa57cb862a7be8c20fa23/e/4440e41e185f4ef3490bb637

bryan_lagrange

See if this helps:

https://cad.onshape.com/documents/84e05fb37e7d6603e0b2b791/w/3bd82f60c470fc671da606ef/e/12319f2e3f0de841ee6a4e0a

S1mon

It's certainly possible to construct this shape in one sketch. There's probably a bunch of ways to do it, but here are the steps I took:

1. Start with the horizontal and vertical centerlines, made them equal and centered on the origin, add the dimension
2. Add a 45 degree centerline by making its end point H+V to the others
3. Add the larger arc (at the top) and made its center aligned to the center line, set the radius, and align the arc to the top end of the vertical centerline, constrain its end points to be mirrored
4. Mirror the top arc around the 45 (adding the left side arc)
5. Add the smaller arc as a tangent arc, and dimension its radius
6. Mirror the left larger arc and smaller arc around the vertical centerline
7. Mirror the top arc and smaller arcs around the horizontal centerline

bryan_lagrange

See if this helps:

https://cad.onshape.com/documents/84e05fb37e7d6603e0b2b791/w/3bd82f60c470fc671da606ef/e/12319f2e3f0de841ee6a4e0a

sam_biddle

This is great.  I'm not quite sure I understand the math, but that's exactly what I was looking for.  Thank you!

bryan_lagrange

Since it is a symmetrical shape I extruded a quarter of the shape and did 2 mirrors to create the entire shape


I created a sketch of the boundary:


I placed the midpoint of the top of the larger radius circle centered with the midpoint of top of the boundary.



I created another larger radius circle and attached the midpoint of the side of the circle with the midpoint of the side of the boundary.



I made a the smaller radius circle tangent with the 2 larger radius circles.



I extruded the upper quarter area



I mirrored the feature twice to get the final shape

sam_biddle

This is VERY helpful.  Thank you!

S1mon

It's certainly possible to construct this shape in one sketch. There's probably a bunch of ways to do it, but here are the steps I took:

1. Start with the horizontal and vertical centerlines, made them equal and centered on the origin, add the dimension
2. Add a 45 degree centerline by making its end point H+V to the others
3. Add the larger arc (at the top) and made its center aligned to the center line, set the radius, and align the arc to the top end of the vertical centerline, constrain its end points to be mirrored
4. Mirror the top arc around the 45 (adding the left side arc)
5. Add the smaller arc as a tangent arc, and dimension its radius
6. Mirror the left larger arc and smaller arc around the vertical centerline
7. Mirror the top arc and smaller arcs around the horizontal centerline

dave_lapthorne

You can easily fix the sketch by applying some tangency constraints between the arc segments and also coincident constraints between the arc end-points