♪Monday, Monday, so good to me ♪♫ … because it is the beginning of another fine SolidWorks week. Over the past two weeks, we have been covering some cool Sketch tools available in SolidWorks 2008. I know some of you might be wondering why I am still in 2008. Well to be honest, I would love to start using 2009 but since my company hasn’t moved to 2009 yet…I am stuck for now. I am working feverishly to work something out to get ‘09 but it may take some time. Until then, I have plenty of topics to cover in 2008 that will still help out those of you who have made the transition to 2009. With that being said, let us just jump right in with both feet…

Close Sketch to Model

This sketch tool can be a great tame saver. The Close Sketch to Model can be used instead of selecting edges on a part and using the Convert Entities tool. Basically, when you create an open profile on a face of a model the Close Sketch to Model tool will close the profile with the existing edges on the model. For this example, I have a sketch created with only a couple of lines and I need to close the profile in order to create the extrusion.

In Tools -> Sketch Tools, select Close Sketch to Model.

Choose Direction to Close Sketch

After selecting Close Sketch to Model, a yellow arrow will be shown at the end of the open sketch showing the direction that the tool will use to close the sketch.

If the direction shown is not what is wanted, selecting Reverse direction to close sketch will flip the arrow in the preview.

Once satisfied with the direction, click Yes will close the sketch.

The sketch segments created with the tool are parametrically linked, meaning that as the model changes the sketch will automatically update.

All that is left to do it to create the extrusion.

Check Sketch for Feature Usage

This tool is not a tool that will help you create a sketches faster, but it will help you make sure the sketch works. Check sketch for feature usage will check the active sketch for any problems that will keep you from creating the feature. While still in your sketch, select Tools -> Sketch Tools -> Check Sketch for Feature…

After selecting the tool you will be presented with a dialog box. The Feature usage field is the the type of feature you intend to make with the active sketch. If the active sketch was already used to create a feature, SolidWorks will automatically select the type of feature created. The Contour type changes depending on the Feature type selected. Each Contour type has its own set of rules that are used to check the viability of the sketch. If the <none> is selected for the Feature usage, the sketch is checked for all errors that are common to all the contour types.

Allowed Contour Types

As mentioned, each feature type has its own contour type that is supported. Below is a list of the available feature types with their corresponding contour types:

• Base Extrude – Multiple Disjoint Closed
• Base Extrude Thin – Single Open, Multiple Disjoint Closed
• Base Revolve – Multiple Disjoint Closed
• Base Revolve Thin – Single Open, Multiple Disjoint Closed
• Boss Extrude – Multiple Disjoint Closed
• Boss Extrude Thin - Single Open, Multiple Disjoint Closed
• Boss Revolve – Multiple Disjoint Closed
• Boss Revolve Thin – Single Open, Multiple Disjoint Closed
• Boundary Surface – Single Open, Single Closed, Multiple Disjoint Closed
• Cut Extrude – Single Open, Multiple Disjoint Closed
• Cut Extrude Thin – Single Open, Multiple Disjoint Closed
• Cut Revolve – Multiple Disjoint Closed
• Cut Revolve Thin – Single Open, Multiple Disjoint Closed
• Jog – Single Open
• Loft Guide – Single Open, Single Closed
• Loft Section – Single Closed
• Mold Parting Surface – General ( The sketch is checked for errors that are common to all contour types)
• Rib – General ( The sketch is checked for errors that are common to all contour types)
• Sketched Bend – General ( The sketch is checked for errors that are common to all contour types)
• SheetMetal Base Flange – Single Open, Multiple Disjoint Closed
• Split Feature – General ( The sketch is checked for errors that are common to all contour types)
• Surface Extrude – General ( The sketch is checked for errors that are common to all contour types)
• Surface Fill – General ( The sketch is checked for errors that are common to all contour types)
• Surface Loft Section – Single Open, Single Closed
• Sweep Path or Guide – Single Open, Single Closed
• Surface Revolve – General ( The sketch is checked for errors that are common to all contour types)
• Sweep Section – Single Open, Multiple Disjoint Closed
• Surface Sweep Section – General ( The sketch is checked for errors that are common to all contour types)

Explanation of the Contour Types

We know what contour types are allowed, but what do the contour types mean? Here is a brief explanation of each contour type:

• General – A feature that allows multiple contour types is marked as General since multiple set of rules apply to the feature creation. When Check sketch for feature usage evaluates the sketch it will check the sketch against a general set of rules that is common among all the contour types.
• Multiple Disjoint Closed – A closed profile can be any set of entities that creates a profile without any gaps. Rectangles and circles are perfect examples of closed contours. A sketch that has multiple closed contours that are disjointed can have more then one circle, for example, that do not touch but can create an extrusion.
• Single Open – A single open contour can be a sketched profile that does not close on itself. Since the profile is open there can not be more then one in a sketch for the selected feature type. An arc, line or spline can be a single open contour, however, spines are not valid for usage as open contours for sheet metal parts.
• Single Closed – A single closed contour is one profile that closes upon itself, such as a rectangle, circle or other sketch.

Select Feature Type

To check a sketch that is not already used to create a feature, select the desire feature from the Feature usage pull-down.

Select the Check button to evaluate the active sketch.

Feature Cannot be Created

If the selected feature cannot be created from the current sketch, a dialog will display the reason for the error.

Sometimes, the messages can be a bit ambiguous but with experience you will be able to determine the issue based on the displayed message.

No Problems Found

Once all the errors in the sketch have been corrected, you will receive the message that no problems were found and the number of contours in your sketch will be displayed. Click the OK button and go ahead with your feature creation.

This is the End…

This concludes our exploration of sketch tools, for now. I am sure that at a later date we will dive back into the subject but for now I am closing the book. Next week will be moving on to another aspect of SolidWorks you may or may not be aware of. Until then… have a happy SolidWorks week!

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