Introduction: Learning a Few Basic Functions of SOLIDWORKS: Making a Six Sided Dice
This Instructable will walk you through the steps required to make a 3D model of a six sided dice.
While designing the model, you will draw on planes and surfaces, extrude and cut 3D shapes, and fillet inner and outer corners or a 3D model.
When working in Solidworks there are often many ways to accomplish the same task. Some will work better for some people than others. With that in mind, the multiple ways you can do some of the steps in this Instructable are not the only way to do this.
Materials required: A computer with Solidworks installed
Time required: 30 min to 1 hour
Step 1: Choosing a Plane to Draw On
Right click on the top plane icon on the left side of the screen. In the picture above, this is indicated by a red arrow
From the menu that appears, click on the option "normal to", as indicated by the yellow arrow. Make note of this icon now, and its general location in this menu, as you will be using this again later.
This rotates the model so that you view the top plane from an angle perpendicular to the plane.
Step 2: Drawing the Base
Next, left click the top plane to select it and then select the sketch tab on the top left of the screen. Doing this should open up the menus as seen on the picture.
Click on the arrow next to the draw rectangle option, this is shown by the yellow arrow.
From the drop down menu appears, find the center rectangle option shown by the orange arrow.
The center rectangle option will draw a rectangle from two clicks. The first click will be the center of the rectangle. The second click will be one of the corners of the rectangle.
For your first click, click the origin, this should be designated in Solidworks by a set of arrows most likely near the center of your screen.
Your second click can be anywhere else on the screen.
Step 3: Setting the Dimensions of the Base
Click on the screen to begin drawing the box as mentioned in the end of step two. Don’t worry about getting dimensions correct during that quick step.
Once the rectangle is drawn, you are going to click on the Smart Dimension icon in the top left, as shown by the red arrow.
Next, click on one of the sides of the rectangle, this will open a dialog box in which you can enter the dimension you want that side to be. Occasionaly you will need to click again to place the dimension before altering the value. Alternatively, you can select the green check in that small box, and enter the dimensions in the left side of the screen. You can do this as well if the box does not appear. The specific area for this is shown by the orange arrow.
When you enter the dimensions, in either area, enter the value "1in"
This will set that side to one inch, regardless of the units it was in before. This may not display in inches. In the picture above it is displaying in meters.
Repeat this smart dimension with the one other side that is perpendicular to the first you chose.
When this is done, exit the sketch via the button on the top left of the screen.
Step 4: Creating the 3D Shape
Select the sketch you have just drawn, and in the features tab in the top left, select extrude base. This is shown by the red arrow.
A yellow shaded region should appear to show you a preview of the 3D shape you are creating through this option.
Select the box shown by the yellow arrow, select the midplane option.
You could select either the bind or midplane options to create the same 3D shape. However, while these will produce the same shape, they will do so by extruding either in one direction, or half as much in two directions. Choosing the midplane option now, will set the origin of the cube to be in the center, making future rotation based steps easier.
In the box shown by the orange arrow, enter the value “1in” again.
When finished select the green check on the left side of the screen. You should have a solid cube now.
Step 5: Drawing the "One Pip" Face
Right click one of the faces of the cube, and select the normal to option again. This menu will have more options than the last, but the normal to option still looks the same as before. For reference, it should be in the top portion of the menu, and the icon is a blue shape with an arrow above it.
Next, select the sketch option in the top left, and then the create circle option, not the perimeter circle option. This is indicated by the red arrow.
Select anywhere in the face of the cube, and click again just a small distance away to create the circle.
Select the smart dimension again. This time you are going to make three smart dimensions.
For the first dimension, select the outside of the circle, shown by the orange arrow, and set the dimension to “0.15in”. Again, you may need to click again to place the dimension before the dialog box opens.
For the second dimension, select any point on the edge of the circle or the center of the circle and either the left or right edge of the cube. The yellow arrows show the positions for this step. Set this value to “0.5in”
For the third dimension, do the same as the second dimension, but with either the top or bottom edges of the cube.
These dimensions are centering the circle in the cube face. When finished exit the sketch the same as before with the button to the top left.
Step 6: Drawing the "Two Pip" Face Part 1
Traditionally, the 1, 2, and 3 sides of the dice are grouped together on sides touching each other. The 6, 5, and 4 sides are opposite of the 1, 2 and 3 sides respectively. For this Instructable I will be following this pattern, however you may chose different orientations if desired.
Hold down the center mouse button and drag the mouse so that you can see another face of the cube. Do not scroll with the center button, just hold it down and move the mouse. Scrolling will zoom in and out.
From this point on you may see past sketches you have done through the cube. Do not confuse these with your current drawing. Any drawing you are bot currently working on will appear grey.
If you use a past sketch to draw on for any step, you will be unable to change the positioning of it through smart dimensions. By drawing on another sketch you are already telling Solidworks where to position the new drawing, and trying to change that with smart dimension will result in an error.
Right click this face and select view normal to again. To begin this drawing select the sketch tab again and this time draw a center line as shown by the red arrows.
This line will go from one corner of the cube to the other, also shown by the orange arrows. Be sure when you click to start and end the line you are on the corners. When you are done with the line hit the escape key or the draw circle option. This is to avoid drawing excess lines.
Next, draw another circle on that line. Be sure that you place the center of the circle on the line. As shown by the yellow arrow.
Finally smart dimension the edge of the circle to “0.15in”, and the center of the circle to the nearest edge of a cube to be “0.25in”.
When you are finished with this step, do not exit the sketch.
Step 7: Drawing the "Two Pip" Face Part 2
Next, while still in the drawing, select the linear sketch pattern option and the circular sketch pattern, as shown by the red arrows.
Select the circle you have just drawn and a preview should appear showing how the pattern will be made.
Next change the number shown by the yellow arrow to the value “2”. This should change the preview to appear like it does in the picture above.
When you are finished with this, select the green check mark, and then exit the sketch.
Step 8: Drawing the "Three Pip" Face Part 1
Rotate the model with the as before with the middle mouse button to view another side.
Again, with step 6, create that same circle along the diagonal line again, and using the smart dimensions give the circle a diameter of "0.15in", and the distance from the closet edge of ".25in".
Now, draw another circle with the same diameter again on the line and smart dimension the center of it to any edge to be "0.5in"
Step 9: Drawing the "Three Pip" Face Part 2
Here you will be creating a circular pattern with the circle not in the center. This will follow the same method as in step 7.
Select the circular sketch pattern as shown by the red arrows.
Select the circle not in the center to rotate, as shown by the orange arrow. At this stage, if the sketch doesn’t rotate around the center, you can fix this by clicking on the same box as before and then the center of the center circle as shown by the green arrows.
Then change the value in the box by the yellow arrow to the value of "2".
When you are done with this, hit the green check mark and then exit the sketch.
Step 10: Drawing and Rotating the "Four Pip" Face
For the fourth side, you will again rotate the device, and create the circle along the diagonal again as you did on the Two Pip face.
This time, however, when you create the circular sketch pattern, you will change the number by the red arrow to be "4" if it is not already.
The preview should look similar to the picture.
When you are done with this, hit the green check and exit the sketch.
Step 11: Drawing and Rotating the "Five Pip" Face
For this face, you will perform the same rotation that you did in step 10. You will also add an additional circle in the center.
The diameter of the circles should be set to "0.15in" like all the rest, and the non-centered circle should be on the diagonal and set "0.25in" from the nearest edge. The center circle is set on the diagonal and "0.5" in from any edge.
When finished, check the green check mark and exit the sketch.
Step 12: Drawing the "Six Pip" Face Part 1
At this point, there should be one face of the cube without any marks on it. Rotate the cube so that you find this side to draw on and view normal to.
In this step, you will not draw the diagonal line again. Instead, start with drawing a single circle somewhere in the top left quadrant of the cube face.
Then smart dimension diameter of the circle to be "0.15in", the center of the circle to be ".3in" away from the left edge, and ".25in" away from the top edge.
Next you will do another sketch pattern, but not the circular pattern you used before, this will be covered in the next step.
Step 13: Drawing the "Six Pip" Face Part 2
Start by selecting the linear sketch pattern as shown by the red arrows. This time you will select the option you have not yet selected in that menu.
This should open up a new menu on the left side of the screen. Now select the circle you have just drawn to create the pattern.
The two boxes indicated by the orange arrows will be where you edit values for this step. If one or more of these values is not visible initially, you can also change the values on the left side of the screen under the corresponding titles. Generally these two boxes will be present if the value under instances is above "1"
For direction 1, change the spacing to “.4in”, and the instances to “2”
For direction 2, change the spacing to “.25in”, and the instances to “3”
If either one of the directions appear to be going in a different direction than intended, you can change this. Depending on which direction is wrong, you can click the button indicated by the green arrows.
When you are done with this step, hit the green check mark, and exit the sketch.
Step 14: Drawing Check
At this point you should have six sketches listed in the left had menu. This is demonstrated by the red box and arrow in the picture.
Don’t worry if your numbers are different than those in the picture. In the event you started a sketch over, deleted an excess sketch, or some other similar reason, the numbers will be different. Solidworks continues to count and label sketches even if you have deleted one.
Step 15: Creating the Pip Holes for a Single Face
For the next step, select only a single one of those six sketches on the left side of the screen by left-clicking on it.
Then in the features tab, select the extruded cut option. This is indicated by the red arrows.
In the menu that appears on the left side of the screen, change the value shown by the yellow arrow, to be “0.075in”. This value is the radius of the circle drawn earlier, and will be used in the later steps to round, or fillet, the holes.
When this is done, click the green check mark again.
Step 16: Creating the Pip Holes for Each Face
Repeat step 15 with each of the six sketches, one by one.
Be sure the depth of each hole is set to be "0.075in"
At the end of this step, each of the six sides should have holes indented in them where you drew the circles earlier.
Step 17: Cut-extrude Check
The six sketches you head earlier should now be six cut-extrudes.
Again, don’t worry about the numbers, so long as each side has been cut-extruded.
Step 18: Selecting the Pip Fillets
Rotate the dice, so that you can clearly see the bottom of each hole made on that side.
Next, select each the bottom face of each of the holes on that side. You can do this by holding shift as you left click each face.
Step 19: Single Face Pip Fillet
With all of the hole faces selected, select the fillet option on the features tab. This is indicated by the red arrow.
Make sure the far left fillet type is selected and that it is set to full preview. The yellow arrows show these portions.
In the box indicated by the orange arrow, put the value “0.075in”.
This will cause the corners to be smoothed out in a circular fashion with the radius of "0.075in". Because you set the depth of the hole to be "0.075 in", and the diameter of the hole to be ".15in", the fillet will form a semi circle.
Click the green check mark when finished with this.
Step 20: Filleting the Remaining Pips
Repeat step 19 for each face of the cube. This can be done one hole at a time, one cube face at a time, or all cube faces at the same time.
If you would like to do all cube faces at the same time, you can hold the shift key down while selecting the faces of the holes. Release the shift key so you can rotate the model, and then hold it down again before selecting more hole faces.
However, when attempting this, you cannot easily deselect a face this way if you accidentally click the wrong one.
Alternatively, you can select the filleting tool before selecting faces to fillet. After selecting the tool, you can then select the features you want to fillet and if you select an incorrect one, it is easier to correct. Simply click the incorrect feature again to deselect it.
Step 21: Filleting the Edges
For this next step you will again use the fillet option.
This time, when using the fillet option, you will select the edges between the dice faces to fillet. Some of these edges are shown by the red arrows on the picture. Do not try to select the faces or the cube as whole, this will change the fillets in the pips. Be careful when selecting the edges to avoid this.
These edges can also be done individually or all together. There are a total of 12 edges to select here.
Next, change the value in the box indicated by the yellow arrow, to be “.05in”
When done with this done, click the green check mark.
Step 22: Finished
You should now have a 3D model of a six sided dice.
In designing this dice, you should have learned the following:
Drawing on a plane
Drawing on a flat face
Extruding a base
Extruding a cut
Filleting a surface
Filleting an edge
By changing the shape, and location of the drawings, most basic 3D model can be produced with this information.
If you would like any further information see the following link:
http://www.solidworks.com/sw/resources/solidworks-tutorials.htm
