Avatech Tricks: Drawing for Dough, Part 17 Oct, 2006 By: Erik Kurek
Useful tips for getting the correct views in Autodesk Inventor.
To paraphrase an old golf saying, "You model for show, but you draw for dough." No matter how well a component is modeled, if the 2D drawing is not readable on the shop floor, then it is useless. Autodesk Inventor provides tools that enable you to transfer ideas from your head to paper. In the first part of this article, I cover broken views, detail views and center lines. In the second part of the article, which will appear next month, I'll cover creating section views and other miscellaneous views.
Figure 1 shows an IDW of the shaft with a base view that I have already placed. The ends of the shaft are hanging over the page on either side.
Figure 1. Shaft with ends off the page.
The Broken View
Inventor's Broken View tool enables me to place the model on my drawing and then cut out the parts I don't want to show. Right-click to view the context menu. After selecting the Broken View tool, a dialog box opens with the option of placing two types of symbols: a structural style, shown as a single jagged line, or a rectangular style, shown as a zigzag line (figure 2).
Figure 2. The Broken View dialog box.
The dialog box also asks for a scale of the breaks, the gap distance and the number of symbols you want to show. After entering the options, pick two points in the view where you would like to break the model, and the view collapses the distance between the first and second picks. To move the symbol, grab the grip in the middle and drag it to a new position. To adjust the break, grab one of the edges of the broken view symbol and drag it away from the other one to make the break bigger, or drag it to the opposite side of the other symbol to make the break smaller (figure 3).
Figure 3. Adjust the broken view symbols by dragging them.
You can place multiple broken views on the same view, adjust the orientation to vertical or horizontal, and when the broken view is dimensioned from one end to the other, the full value of that distance is shown. Your dimension style will show the break symbol on the dimension line if that option is chosen.
The Detail View
Inventor's Detail View tool can show a larger area so that the dimensions look cleaner and the drawing is easier to read. Right-click in the view, choose Create View / Detail and the Detail View dialog box opens. The dialog box enables you to change the label, scale, style and type. Inventor asks for a center point and another point to define the detail view circle.
Figure 4. The Detail View dialog box.
Once the view is placed in the IDW, you can adjust the location of the symbol by dragging it around the detail circle; you can adjust the size and location of the circle by dragging the grips. To keep the detail circle locked to a particular area if the model changes, right-click on the view symbol and select the Attach option. The detail view also has a rectangular fence option that is created the same way.
Inventor automatically generates the next label letter in the list based on the last letter placed in the drawing. The software also sets the scale of the detail to twice the value of the parent view (figure 5). You can move the label letter to any point on the detail view symbol to keep it out of the way and readable.
Figure 5. The Detail View shows the difference in the edges.
Adding Center Lines
Now I want to add some annotation to these enlarged views shown above. Generally I want to place some linear diameter dimensions on Detail P to the left. These types are generally shown with only one-half of the dimension visible and usually dimensioned about the center line. This process used to be time-consuming and resulted in static dimensions that didn't adjust with the model, leaving room for potential manufacturing mistakes and costly errors.
To get the center line from geometry that is trimmed out, right-click inside Detail P view and select Automated Centerlines. In the dialog box, make sure that you apply the center lines to the right objects -- usually I choose holes, cylindrical objects and revolved objects -- and that the Objects in View, Axis Parallel button (see the blue arrow in figure 6) is selected to show side-view center lines. You can also adjust the threshold of the item so that really small or really large fillets and circular edges do not get a center line placed on them.
Figure 6. Make sure the Objects in View, Axis Parallel button is selected in the Automated Centerlines dialog box.
The center line of the revolved geometry now shows below the view. You can use that center line to place linear diameter dimensions. Use the General Dimension tool to select the first and second points. It is usually better to select whole lines or edges than points, especially the center line. Before placing the dimension text, right-click and select Dimension Type / Linear Diameter. It is important that the type is chosen before placing the text because once it is placed, there is no way of changing the type except for erasing it and placing another text item.
As dimensions are placed, the dimension and extension lines for the other half are turned off. Since this part is a round, a diameter symbol is also shown as part of the text. If you find selecting the edge difficult, zoom in with your middle mouse wheel so that you can select the line better and use the F5 key on your keyboard to take you back to the previous view. When finished, turn off the visibility with a right-click on the line.
Next month I'll continue this topic by discussing section views and other miscellaneous views.
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