Dimensioning with Equations

Parametric Modeling: Dimensioning with Equations Page 7 of 10

Dimensioning with Equations

Parts are often designed as a set or Family of Parts. They are based on one Part, but may have difference sizes. For example, if designers were making a set (family) of pipe fittings, they would not design each part. They would design one part and base the other parts on that one.

The easiest way to make a Family of Parts is with Equations. Equations can be used to dimension model features and establish relationships between model geometry. When select Dimensions are edited, they will have a predictable effect on related parts of the model. This saves a lot of time during modeling process.

Legos® are a good example of a Family of Parts. A brick has certain design properties which do not change. However, parts of the Legos® must change when the size increases.

Procedure

Open a new Standard.ipt file. Choose Two-point Rectangle from the Sketch Toolbar. Sketch a Rectangle approximately 5/8” (0.625) x 1-7/8” (1.875).

Choose General Dimension from the Sketch Toolbar and place a depth dimension on the left edge. See Figure1.

Look above the Dimension and notice the dimension’s name is d0. This Dimension will be referred to several times throughout the remainder of this exercise. Enter 0.625 as the depth for d0.

Figure 1

Place a Dimension on the width. As the dimension box appears, notice the name given: d1. As each Dimension is placed, Inventor creates a new Variable name for it.

Write the following Equation in the Dimension Field (d0 * 6) / 2 in (See Figure 2) and Press the Check Mark. Notice that the Dimension for d1 becomes fx:1.875.

Figure 2

Next, Right click in the graphics window and choose Done. Right click and choose Isometric View. Finally, Right click again in the graphics window and choose Finish Sketch.

Choose Extrude from the Features Toolbar. In the Extrude Dialog Box, set the distance to 0.375 and click OK.

Shelling the Brick

Choose the Rotate toolfrom the Standard Toolbar and rotate the part so you can see the bottom.

Choose Shell Tool from the Features Toolbar. Click the bottom face of the part to have it removed, when the Shell feature is finished. Set the thickness to 0.05. Make sure the Inside Shell and the Remove Face Buttons are depressed, place the cursor on the face shell out and click OK. See Figure 3.

Figure 3

Creating the Pegs

Create a Sketch Plane on the top of the part. Choose Center Point Circlefrom the Sketch Toolbar. Sketch the circle in the lower left corner.

Choose General Dimension from the Sketch Toolbar and place a Diameter Dimension on the circle of 0.2 inches.

Did you notice that this circle is d5? That’s because d2 was the extrusion to .375 (height), d3 was a 0 degree taper angle that goes with extrude and the shell to .05 was d4.

Figure 4

Place a location dimension on the front edge to the center of the circle. Write the following Equation in the dimension field: d0 / 4 and press the Check Mark. Notice that the dimension d6 becomes 0.15625. (Because of the preset viewing precision, the Dimension appearing on the sketch will round to .156.)

Do the same for the side edge to the center of the circle—this becomes d7. See Figure 5.

Figure 5

Finish the sketch and Extrude the circle up (Join) 0.075 inches.

Choose the fx Parameters iconfrom the Part Features Toolbar. This will bring up a Spreadsheet of the values of the variable which have been used to this point.

In the dialog box, under the Comment column, type in the labels as shown in Figure 6 below. Click Done when finished placing all the comments.

Figure 6

NOTE: Labeling is a good design practice. It reminds the designers what each variable represents in their model. Commenting on the variables, as was shown here, should be done throughout the rest of the exercise. Do not wait till the end to label them all.

Choose Filletfrom the Features Toolbar. In the dialog box, change the Fillet Radius to 0.002. Now Click the top edge of the peg to add a round to it. Click OK. See Figure 7.

Figure 7

Renaming a feature

In the Browser, under the modeling section, Right click on Extrusion 1 and select Properties.Change the name to Brick Extrusion. Click OK. See Figure 8.

Figure 8

In the Browser, Click the + sign next to Brick Extrusion to open its folder.Left click on the Sketch, Left click a second time, and change the name to Brick Sketch. (This may take a couple of tries and double clicking, in order for the space name to be changed.) Click OK.

At the top tool bar, choose the Update button. This will make the model active again.

In the Browser, change the names of all the items to match Figure 9 at right.

Figure 9

NOTE: Once again, labeling is a good design idea. It clarifies the steps taken.

Replicating the Pegs

Choose Rectangular Pattern from the Features Toolbar.

In the Browser, click on the Peg Extrusion and Peg Round. (Holding the shift button down as one is making the selection keeps both.) See Figure 10.

Figure 10

In the dialog box, click on the Direction 1 arrow and choose the front edge.

Make sure that the arrow that appears points down along the length of the edge. If not, click Flip Directionto change the direction of the pattern.

Change the Count to (d1/d0)*2 and the Spacing to d0/2.

See Figure 11.

Figure 11

In the dialog box, click on the Direction 2 arrow and choose the top edge. Again, if the arrow points in the wrong direction, change it so that it goes towards the back.

Set the Count number at 2 and change the Spacing to d0/2. See Figure 12 at right.

Click OK.

Figure 12

Create the “dimples” inside the Lego block

Choose the Rotate toolfrom the Standard Toolbar and rotate the part so you can see the bottom.

Choose the Look At toolfrom the Standard Toolbar and choose the inside of the part.

Create a Sketch Plane on the inside bottom of the part. Double check this by rotating the part to be sure the Sketch Plane is on the inside bottom and nowhere else.

Choose Center Point Circle from the Sketch toolbar. Sketch the circle in the upper left (front) corner.

Choose General Dimensionfrom the Sketch toolbar and place a Diameter Dimension on the circle of 0.1.

Place a location Dimension on the front edge to the center of the circle. Write the equation d0/4 in the dimension field and press the Check mark.

Do the same for the top edge to the center of the circle. See Figure 13.

Finish the Sketch and choose the profile of the circle to Extrude as a cut 0.025.

Figure 13

NOTE:This would be a good point to label the items in the Parameters dialog box and the Browser.

Replicate the Dimple Pattern

Choose Rectangular Pattern from the Features Toolbar. In the Browser, click on the dimple Extrusion.

In the dialog box, click on the Direction 1 arrow and choose the front edge. Make sure that the arrow that appears points down along the length of the edge. If not, click Flip Directionto change the direction of the pattern.

Change the Count to (d1/d0)*2 and the Spacing to d0/2.

In the dialog box, click on the Direction 2 arrow and choose the top edge. Again, be sure that the direction indicated is correct.

Keep the Count as 2 and change the Spacing to d0/2. Click OK. The inside dimples have now been created.

Create the Locating Column

Create a Sketch Plane on the inside bottom of the part.

Choose Center Point Circlefrom the Sketch toolbar. Sketch a circle and place a Diameter Dimension of 0.25. (See figure 16 for approximate circle placement.)

Place a location Dimension on the OUTSIDE front edge to the center of the circle. Write the equation d0/2 in the Dimension field and press the Check mark.

Figure 14

Do the same for the OUTSIDE top edge to the center of the circle.

Finish the Sketch and choose the Profile of the circle to Extrude it 0.325.

Create a Sketch Plane on the bottom (the upper-most face in the sketch) face of the column. Choose the Point, Center Point tool and click the center of the circular face to create a center mark. Finish the Sketch.

ChooseHole from the Features toolbar, then select the center mark on the column face you just created.In the dialog box, change the Diameter of the Hole to 0.2 and the Distance to 0.325. Choose Flat for the Drill Point. Click OK. See Figure 15.

Figure 15

Choose the Fillet toolfrom the Features toolbar. In the dialog box, change the Fillet Radius to 0.002. Now click the inside edge of the column to add a round to it. Click OK.

NOTE: This would be a good point to label the items in the Parameters Dialog Box and the Browser!

Replicate the Support Column

Choose the Rectangular Patternfrom the Features toolbar.

In the Browser, click on the Column Extrusion, Column Hole and Column Round (Remember to hold the shift key to choose all three). Isn’t is easier to identify the features by naming them?

In the dialog box, click on the Direction 1 arrow and choose the front edge.

NOTE: You may need to click the Flip Directionto change the direction of the Pattern.

Change the Count to (d1/d0)*2)-1 and the Spacing to d0/2.Click on Direction 2 and click on the side edge. Be sure the direction is correct and change the Count to 1.

Click OK.

Create a Rib Extrusion

Click the Look At icon at the top toolbar then create a Sketch Plane on the inside bottom of the part.

Choose Two-Point Rectanglefrom the Sketch toolbar. Sketch a rectangle connecting the inside walls together. Click Done.

Place a width Dimension of 0.025. To create the location Dimension on the OUTSIDE top edge to the left edge of the rib, type in the Equation d0 -0.0125 in the Dimension field and press the Check Mark. See Figure 16.

Finish the sketch and choose the Profile of the rectangle to Extrude 0.25.

Figure 16

NOTE: This would be a good point to label the items in the Parameters Dialog Box and the Browser.

You probably noticed that the Rib Extrusion is going through the Column Hole (Figure 17).

This can be corrected by editing the order of the features in the Browser. Click and Hold on the Rib Extrusion in the Browser. Now drag it up above the Column Extrusion. See Figure 18.

Figure 17- Before Figure 18 - After

Choose Rectangular Patternfrom the Features toolbar.In the Browser, click on the Rib Extrusion.

In the dialog box, click on the Direction 1 arrow and choose the front edge.

Change the Count to (d1/d0)-1 and the Spacing to d0. This time do not pick a second direction. Notice the preview before clicking OK.

Once again, the Rib Rectangular Pattern is going through the Column Hole. This can be corrected by editing the order of Pattern in the Browser. Click and Hold on the Rib Rectangular Pattern in the Browser. Now drag it just below the Rib Extrusion.

Before After

Label the remainder of items in the Parameters dialog box and the Browser. Save this file as Lego 6 long.ipt

Create a New Part

Open the Parameters dialog box and change the Equation for d1 to (d0 * 10 in) / 2. Click Done.

Choose Update from the Command toolbar. Rotate the part to see that all the Features have increased. Compare this part to the previous part. This is the power of parametric modeling! Save this file as Lego 10 part.ipt

Lego challenge: Create more parts like those above. You may need to change or delete some of the features in the Lego® to make the smaller sizes.

Mr. Cook Introduction to Engineering Project Lead the Way