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Annotate a drawing with centerlines and dimensions.
Type:
Tutorial
Length:
6 min.
Tutorial resources
These downloadable resources will be used to complete this tutorial:
Transcript
00:03
In this tutorial, you annotate a drawing with centerlines and dimensions.
00:09
With the Flanged-Collar.dwg file opened to the sheet view, on the ribbon, Annotate tab, Symbols panel, click Centerline Bisector.
00:19
Select two lines in each detail view to indicate the centerline of the cylindrical portion of the view.
00:27
Now, from the Annotate menu, click Center Mark,
00:32
and then select the overall diameter in the Top view and the hole centers in the Front and Right views.
00:42
Next, from the Annotate menu, click Centerline, and select the hole centers of the hole pattern in the top view to create a radial center line.
00:52
Right-click to open the Marking menu and click Create to complete the command.
00:58
You can edit center lines by simply selecting the end points of the center lines
01:03
and dragging them to the distance you require from the drawing view.
01:09
You can now start placing some dimensions.
01:13
On the ribbon, Annotate tab, Dimension panel, select Dimension.
01:17
When you select one of the edge lines,
01:20
notice that the diameter symbol is automatically added to this particular dimension, based upon the selection.
01:27
Click OK to close the Edit Dimension dialog.
01:31
With the General Dimension command still active, click to place a couple of additional dimensions,
01:36
one on the top and another one on the bottom.
01:42
Place another dimension for the inside diameter of the groove detail by selecting the two edge end points.
01:53
Notice for this dimension that a no diameter symbol appears.
01:58
From the Edit Dimensions dialog, Text tab, locate the cursor at the start of the text string,
02:03
then select the diameter symbol to add it to the dimension, and then click OK.
02:09
Right-click the graphic window and click OK to finish the General Dimension command.
02:16
Next, you can create multiple ordinate dimensions in a single process.
02:22
On the ribbon, select Ordinate Set from the drop-down.
02:27
In the Section view, click to select a datum point, then click to select the vertical edge to locate the dimensions.
02:34
Right-click and choose Continue, then click to place the dimensions.
02:39
Right-click and select Done to accept the dimensions and end the command.
02:44
Moving to the Detail view, right-click in an open space and, from the Marking menu, select General Dimension.
02:53
Select two end points for the width of the groove slot.
02:59
In the Edit Dimensions dialog, on the Precision and Tolerance tab, select a Tolerance Method of Deviation,
03:07
and set the Upper tolerance value to +0.05 mm.
03:13
Create a depth a dimension for the same slot and set the Deviation tolerance to +0.02 mm.
03:24
Click OK, then right-click and select OK from the Marking menu.
03:29
Move to the Top view, where you can create several different types of dimensions.
03:33
Right-click and, from the Marking menu, select General Dimension.
03:39
Place two linear dimensions from the center to the edge of the boss feature.
03:52
Click OK.
03:56
With the General Dimension command still active, select the center line of one of the hole features and the center line of the part.
04:04
Notice that an angular dimension is created.
04:08
Click OK.
04:11
Now select a radius on the boss feature and add a radius dimension.
04:16
Click OK.
04:19
All of these dimensions are created as you go, and you do not have to cancel the command to switch to a different type of annotation.
04:28
On the ribbon, Annotate tab, Feature Notes panel, click Hole and Thread.
04:34
Select the tapped hole to place the tap dimension.
04:39
Right-click and select OK.
04:42
You can get model dimensions and display them within the drawing environment.
04:46
In the Right view, right-click and in the Marking menu, select Retrieve Model Annotation.
04:53
In the Retrieve Model Annotation dialog, click Select Dimension Source.
04:59
Select the 7-millimeter diameter hole feature, and again click Select Dimension Source.
05:07
Click OK.
05:09
Then, Right-click this dimension, and from the shortcut menu, select Edit Model Dimension.
05:15
In the Hole Dimensions dialog, set the Hole Diameter to 6 mm.
05:21
Click OK.
05:23
This change is saved to the 3D model.
05:26
You can continue adding dimensions to this drawing to finalize the detailed view.
05:32
Once you have completed adding dimensions to this drawing, make sure that you save your progress.
Video transcript
00:03
In this tutorial, you annotate a drawing with centerlines and dimensions.
00:09
With the Flanged-Collar.dwg file opened to the sheet view, on the ribbon, Annotate tab, Symbols panel, click Centerline Bisector.
00:19
Select two lines in each detail view to indicate the centerline of the cylindrical portion of the view.
00:27
Now, from the Annotate menu, click Center Mark,
00:32
and then select the overall diameter in the Top view and the hole centers in the Front and Right views.
00:42
Next, from the Annotate menu, click Centerline, and select the hole centers of the hole pattern in the top view to create a radial center line.
00:52
Right-click to open the Marking menu and click Create to complete the command.
00:58
You can edit center lines by simply selecting the end points of the center lines
01:03
and dragging them to the distance you require from the drawing view.
01:09
You can now start placing some dimensions.
01:13
On the ribbon, Annotate tab, Dimension panel, select Dimension.
01:17
When you select one of the edge lines,
01:20
notice that the diameter symbol is automatically added to this particular dimension, based upon the selection.
01:27
Click OK to close the Edit Dimension dialog.
01:31
With the General Dimension command still active, click to place a couple of additional dimensions,
01:36
one on the top and another one on the bottom.
01:42
Place another dimension for the inside diameter of the groove detail by selecting the two edge end points.
01:53
Notice for this dimension that a no diameter symbol appears.
01:58
From the Edit Dimensions dialog, Text tab, locate the cursor at the start of the text string,
02:03
then select the diameter symbol to add it to the dimension, and then click OK.
02:09
Right-click the graphic window and click OK to finish the General Dimension command.
02:16
Next, you can create multiple ordinate dimensions in a single process.
02:22
On the ribbon, select Ordinate Set from the drop-down.
02:27
In the Section view, click to select a datum point, then click to select the vertical edge to locate the dimensions.
02:34
Right-click and choose Continue, then click to place the dimensions.
02:39
Right-click and select Done to accept the dimensions and end the command.
02:44
Moving to the Detail view, right-click in an open space and, from the Marking menu, select General Dimension.
02:53
Select two end points for the width of the groove slot.
02:59
In the Edit Dimensions dialog, on the Precision and Tolerance tab, select a Tolerance Method of Deviation,
03:07
and set the Upper tolerance value to +0.05 mm.
03:13
Create a depth a dimension for the same slot and set the Deviation tolerance to +0.02 mm.
03:24
Click OK, then right-click and select OK from the Marking menu.
03:29
Move to the Top view, where you can create several different types of dimensions.
03:33
Right-click and, from the Marking menu, select General Dimension.
03:39
Place two linear dimensions from the center to the edge of the boss feature.
03:52
Click OK.
03:56
With the General Dimension command still active, select the center line of one of the hole features and the center line of the part.
04:04
Notice that an angular dimension is created.
04:08
Click OK.
04:11
Now select a radius on the boss feature and add a radius dimension.
04:16
Click OK.
04:19
All of these dimensions are created as you go, and you do not have to cancel the command to switch to a different type of annotation.
04:28
On the ribbon, Annotate tab, Feature Notes panel, click Hole and Thread.
04:34
Select the tapped hole to place the tap dimension.
04:39
Right-click and select OK.
04:42
You can get model dimensions and display them within the drawing environment.
04:46
In the Right view, right-click and in the Marking menu, select Retrieve Model Annotation.
04:53
In the Retrieve Model Annotation dialog, click Select Dimension Source.
04:59
Select the 7-millimeter diameter hole feature, and again click Select Dimension Source.
05:07
Click OK.
05:09
Then, Right-click this dimension, and from the shortcut menu, select Edit Model Dimension.
05:15
In the Hole Dimensions dialog, set the Hole Diameter to 6 mm.
05:21
Click OK.
05:23
This change is saved to the 3D model.
05:26
You can continue adding dimensions to this drawing to finalize the detailed view.
05:32
Once you have completed adding dimensions to this drawing, make sure that you save your progress.
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