Help to create a gear
Hi guys. Im a bit stuck, I have provided you with the drawing. I just seem to cant get the bent part to be radius 7 on all.
I will also upload my part file so you can see how it is atm.
Try to sketch it like this.
You'll also want to make sure your arcs are tangent to the lines, and to each other.
I'd add a single hole for each of the other features, and then use a circular pattern to get the remaining ones. It looks like you may have used a patterned sketch instead. Both will work, but keeping each sketch as simple as possible makes later edits much easier. If someone asks you to change the shape of the holes, you are screwed. Changing a single instance of a shape in a sketch is a lot easier.
Your later sketches look correct but should be fully defined with dimensions.
I dislike the use of contour selection when making features as it allows for poor sketching habits. Cut Extrude 10 uses the contour option
My model is made in SolidWorks 2016 so you won't be able to open it with SW2015. The radius of each bend is 7, but one is an inside radius and the other is an outside radius. You can import the Step file and see how it looks though.
Start over and duplicate the shape and dimensions in my sketch. I think if you try to fix yours, it will only be more confusing as you are missing the tangent relationships and some of your dimensions are questionable. For example, your "33" is calling out the length of a line. It should go to the center of the radius. It is a small distinction that goes away once the correct dimensions and relationships are added, but starting out with a line length can lead to problems.
If I try to fix your existing sketch I get this result (see attached image). Please zoom in and see how the center points of the arcs are not on top of each other. Again, it is a small difference.
It looks better. I think it is still missing one tangent relationship between the two upper arcs, but you solved that with another 5mm dimension.
The vertical line on the left is still blue and needs to be the outside diameter of the part (160mm).
An easier way to draw the sketch is to make use of the Offset command. See attached image. Then you only have to deal with half of the dimensions and constraints.