SolidWork 2013 - Modifying Tool - How To Move, Rotate, Copy, Past, Scale And Split

Moving Sketched Entities

CommandManager: Sketch > Move Entities

SolidWorks menus: Tools > Sketch Tools > Move

Toolbar: Sketch > Move Entities

The Move Entities tool in the Sketch CommandManager is used to move an entity from one location to other.

To move an entity, invoke this tool from the Sketch CommandManager or select the entities, right-click, and then choose the Move Entities option from the shortcut menu. Remember that this tool will be available only when at least one sketched entity is drawn. When you invoke this tool, the Move PropertyManager will be displayed and you will be prompted to select the sketched items or the annotations to be moved. The options in this PropertyManager are discussed next.

Entities to Move Rollout

The options in this rollout are used to select the entities to be moved. You will notice that the Sketch items or annotations selection box is active in this rollout. The names of the entities selected to be moved will be displayed in this selection box. To remove an entity from the selection set, select it again from the drawing area.

Alternatively, you can select its name from the Sketch items or annotations selection box and right-click to display the shortcut menu. Choose the Delete option from the shortcut menu. If you choose the Clear Selections option from the shortcut menu, all the entities in the selection set will be removed.

You will notice that by default, the Keep relations check box is cleared. If you move the sketched entities with this check box cleared, the relations applied to the entities to be moved will be removed. If you select this check box and then move the entities, then the relations applied to the sketched entities are retained even if you move the entities.

Parameters Rollout

The Parameters rollout is used to specify the origin and destination positions of the entities selected to move. The options in this rollout are:

From/To

The From/To radio button is selected by default. So, you can move the selected entities from one point to another.

To move the selected entities using this option, click once in the Base point selection box; you will be prompted to define the base point. Click anywhere in the drawing area to specify the base point; a yellow circle will be displayed where the start point is specified and you will be prompted to define the destination point. Select a point anywhere in the drawing area to place the selected entities.

X/Y

The X/Y radio button is selected to move the selected entities by specifying the relative coordinates of X and Y.

On selecting this radio button, the Delta X and Delta Y spinners will be displayed below this radio button. Set the values of the destination coordinates in these spinners with respect to the current location.

Repeat

If the Repeat button is chosen, the entities will move further with the incremental distance specified in the Delta X and Delta Y spinners.

Rotating Sketched Entities

CommandManager: Sketch > Move Entities flyout > Rotate Entities

SolidWorks menus: Tools > Sketch Tools > Rotate

Toolbar: Sketch > Move Entities flyout > Rotate Entities

To rotate the sketched entities, choose the Rotate Entities tool from the Move Entities flyout in the Sketch CommandManager.

Alternatively, select the entities and right-click to display the shortcut menu. Then, choose Rotate Entities from the shortcut menu; the Rotate PropertyManager will be displayed and you will be prompted to select the sketched items or annotations.

Select the entities to be rotated; the names of the selected entities will be displayed in the Sketch items or annotations selection box of the Entities to Rotate rollout. Next, click in the Base point selection box in the Parameters rollout; you will be prompted to specify the center point of rotation. As soon as you specify the center point, the Angle spinner in the Parameters rollout will be highlighted. You can specify the angle of rotation using this spinner. You can also drag the mouse on the screen to define the angle of rotation.

Scaling Sketched Entities

CommandManager: Sketch > Move Entities flyout > Scale Entities

SolidWorks menus: Tools > Sketch Tools > Scale

Toolbar: Sketch > Move Entities flyout > Scale Entities

To resize the entities, choose the Scale Entities tool from the Move Entities flyout in the Sketch CommandManager.

You can also select the entities and right-click to display the shortcut menu. Next, choose Scale Entities from the shortcut menu to invoke this tool; the Scale PropertyManager will be displayed and you will be prompted to select the sketched items or annotations.

Select the entities to be resized; the names of the selected entities will be displayed in the Sketch items or annotations selection box of the Entities to Scale rollout. After selecting the entities to be scaled, right-click; you will be prompted to specify the point about which to scale. Specify the base point in the drawing area by clicking the left mouse button. After specifying the base point, specify the magnification factor in the Scale Factor spinner of the Parameters rollout. The entities will be resized based on the value set in this spinner. If you need to create the copies of the selected entities, select the Copy check box. Else, choose the OK button from the Scale PropertyManager; the selected entities will be resized. On selecting the Copy check box, the Number of Copies spinner will be displayed. Set the number of instances in this spinner and choose the OK button from the Scale PropertyManager; the entities will be resized and their copies will be created with an incremental scale factor with respect to the original entities selected.

Copying and Pasting Sketched Entities

CommandManager: Sketch > Move Entities flyout > Copy Entities

SolidWorks menus: Tools > Sketch Tools > Copy

Toolbar: Sketch > Move Entities flyout > Copy Entities

The Copy Entities tool allows you to copy the selected sketched entity and paste it to other location. Note that if dimensions are also selected along with the entities to be copied, then the dimensions will also be copied along with the sketched entities.

To copy and paste the sketched entities, choose the Copy Entities tool from the Move Entities flyout in the Sketch Command Manager; the Copy PropertyManager will be displayed. Select the entities that you want to copy and then select the From/To

radio button, if it is not selected by default. Next, click once in the Base point selection box and then specify the base point. Now,

move the cursor; you will notice that the preview of the entities to be copied will be attached to the cursor. Click at a location in the drawing area to place the copied entities. If you need to create multiple copies, left-click at different locations. Else, right-click to invoke the shortcut menu and then choose the OK option from it to exit the tool.

On selecting the X/Y radio button in the Parameters rollout of the Copy PropertyManager, you need to specify the X and Y coordinates of the new entities with respect to their current location and choose the OK button. Note that on selecting the X/Y radio button, you cannot create multiple copies of the selected entities.

Splitting Sketched Entities

CommandManager: Sketch > Split Entities (Customize to add)

SolidWorks menus: Tools > Sketch Tools > Split Entities

Toolbar: Sketch > Split Entities (Customize to add)

The Split Entities tool is used to split a sketched entity into two or more entities.

To split an entity, invoke the Split Entities tool from the Sketch CommandManager; the Split Entities PropertyManager will be displayed. Move the cursor to a location from where you want to split the sketched entity. When the cursor snaps to the entity, press the left mouse button to add a split point. Next, right-click to display the shortcut menu and then choose the OK option from the shortcut menu. Select the sketched entity using the select cursor. You will notice that the sketched entity is divided in two entities and a split point is added between the two sketched entities. You can add as many split points as you need.

Remember that to split a circle, a full ellipse, or a closed spline, you need to split them at least at two points.

You can also delete the split points to convert a split entity into a single entity. To delete a split point, select the split point and press the DELETE key. You can also right-click on the split point to display the shortcut menu, and then choose the Delete option from it.