Create GROOVE & LIP in pairs Product

See you again in the  Solidworks Tutorial. Long we did not do an update. Hopefully, all readers can apply the Solidworks program is well. This time I want to raise the topic of how to make the LIP and GROOVE. If you do not know what a lip and groove, let the reader look at this picture about the product of body and cover. The examples of Lip and Groove  can also be found on the  tv remote, mobile phone, telephone, etc.
Well we just started learning. First I would like to specify the products that I make. Call it an energy efficient lighting products that consist of body and glass cover. In the early stages I will make one body and glass cover unity.

1. Revolved BOSS/BASE

• In the Feature Manager select Front Plane and left click

• Then point your cursor on the Feature Toolbar and select Revolved Boss / Base or select Insert > Boss / Base > Revolve

• Create a sketch of the drawing to be as shown below

• You can use the sketch toolbar menu and select arc and line to create the drawing above.

• Then put the size or dimension through the sketch toolbar and select smart dimension.

• For R6 and R40 choose fillet sketch on sketch toolbar

• Exit Sketch

• Will appear dialog box Revolve-Thin1.

Under parameter Axis of Revolution, click on the blue line as Axis.

Check the Thin Feature then write T1 with numbers  2.00mm  and click Reverse Direction on Type One Direction under Feature Thin parameters.

• Click OK

2. SPLIT 

• Point the cursor on the Feature Manager and click Top Plane.

• In the Feature toolbar choose Split. Split1 dialog box will appear.

• Under Trim Tools parameters  the Top Plane that we were going to be clicking automatically became Trimming Surface. Then click Cut Part below.

• Body will be divided into two that is number 1 and 2. Check one box. Suppose we check the box first, then the Body 1 would change color to magenta.

• Click OK

3. LIP / GROOVE
Next we will go directly to the discussion topic that makes lip / groove. In order to view lip / groove that we will create later appeared highly visible, we can cut a part into two sections with the Section View command. Choose the Front Plane in the Feature Manager and click on the picture toolbar Section split pipe or View> Display> Section View. So it will look like the drawing below.

• Then choose Lip / Groove icon on the menu or Insert> Feature Fastening> Lip / Groove, it will display a dialog box LipGroove2-Groove.

• Under parameter Body / Part Selection choose the body to be made of his groove. In this case select the upper body of conical (Split1 [1])

Then choose the body to be made of his lip. In this case select the lower body that form of a half circle (Split1 [2])

Next, still under parameter Body / Part Selection choose Top Plane in the Feature Manager

• Furthermore, under the parameter Groove Selection command, there are two options namely "face selection and edge selection". When we had to choose Top Plane as 'planar face' the surface to be our 'groove' will automatically be selected by itself. Now we stay moving box below to select or choose the 'edge' (end / edge) of the areas that are 'groove'. Click on the inner edge. When we did the "Groove Selection", the bottom part will be hidden so that only the upper part only visible part. This is the fun of using SolidWorks.

• Further! Under Lip Selection parameter which also contained two boxes of selection options, then the surface will be given lip commands will automatically be selected as the Top Plane as its planar face.

Go to selection box below and click, then the upper part turn will be hidden. Now that looks are the lower body. Then click the 'edge' as the inside of the lip area.

• The final step is to determine the value of groove and lip Parameters that can you see in the picture above at the lower left.

• Click OK

Don't forget to click the Section View to restore the drawing as a whole. Good luck!