Soldiworks:cutting a notch around a radius 1

[mikek1217]

Hi. This is my first post. I am a new Solidworks user. I have modeled a plastic molded part and am having trouble cutting a notch into the top surface. Basically, the section of the part I an having trouble with has a straight then a radius then another straight. This section of the part is 2" wide. I want to cut a notch .030 deep x .50 wide in the middle of this section. How do I cut this notch around the radius? Thanks.

 

[SBaugh]

If it's a straight cut then offset a plane of pick the falt face and make your profile and cut it. If it requires a sweep then make yout path and profile and cut it.

Either way I don't truly follow what the situation is because your a little vague about the whole process and what your looking at.

If you have the ability to post images post them here or links to them.

Also sounds like you need to go through the Online tutorial. This will help explain a lot about basic part designing.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

There are a couple of ways:-
1) Cut Sweep;
Create a plane where you want the notch to start.
Start new sketch on the plane & draw a profile then close the sketch.
Create another plane perpendicular to the first plane, start a new sketch, draw the path (consisting of line-arc-line) that you want the profile to follow then close the sketch.
Use Insert > Cut > Sweep to cut the notch.

2) Thicken Surface;
Create a surface on the faces where you want the notch cut into, then Insert > Cut > Thicken the surface to create the notch.

 

[Mandrake22]

I will assume that the "straight" sections are also flat.
First, make sure that the part has been modeled with the initial sketch centered about the origin. Open a new sketch on the plane that bisects the desired notch.Select the straight edges and the radius on one edge or the other and click the "Convert Entities" button and. This will copy these entities to the centerline sketch plane. Click the "Offset Entities" button and select these newly copied entities and select .030" as the offset value and be sure to click on the inner side to define the direction of offset. Draw lines at the ends of this new sketch to close it off. Do an extruded cut and be sure to select "Mid Plane" as direction 1. Admire handiwork!
If your notch isn't centered on the part you will have to create a new plane at the location of the center of the notch or at either edge of it. This plane is required to create a "landing spot" for the "Convert Entities" function.

 

[mikek1217]

CorBlimerLimey,
Your cut sweep instructions worked perfectly. I will use cut sweep often. Thanks for helping out a new user.

Regards,
Mikek12217

 

[CorBlimeyLimey]

mikek1217 ... You should also practice with the other methods mentioned by myself & Mandrake22. Each have their time & place to be used. Actually Mandrakes method is probably the easiest to use & is best for file size.