To Trim or Extend a Chain
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This topic discusses chain modification while working inside of a tool and using the Chain dialog box. If you want to modify a chain while working outside of a tool, you can use the SHIFT key to clear the selection of individual items from the ends of a chain or use the CTRL key to remove an entire chain from the selection set. Refer to About Selection under See Also for more information about clearing a selection.
You can trim or extend open-ended chains (One-by-One, Tangent, and Partial Loop).
You can trim closed-loop chains but you cannot extend them.
1. Construct the chain and open the tool in which to work with the chain, or select a feature that contains an existing chain that you want to modify and click Edit Definition.
2. Locate the Detail collector that contains the chain that you want to modify. Detail collectors are located on the panel. Note that you cannot use the Summary collector (located on the dialog bar) to modify a chain.
3. Click Details. Creo Parametric pauses the tool, opens the Chain dialog box, and displays the attributes for the chain.
4. If the panel Detail collector contains more than one chain, select the chain to modify from the chain list in the Chain dialog box. The chain attributes are displayed.
5. Click the Options tab. If you have selected a closed-loop chain, then the Start Point check box appears selected by default.
6. For closed-loop chains, if required, modify the start point using the Start Point collector and the Flip button. Clear the Start Point check box. The options under Length Adjustment become available.
7. To trim or extend End 1 or End 2 of a chain, use one of the following options under Length Adjustment:
Value—Trim or extend a chain using a value. Type a distance value and press ENTER, or select a most recently used value from the list. Note that negative values trim a chain. You can also drag the handle on your model to adjust the value. To add a relation to a feature for the extend values of chain ends when creating or redefining a feature, perform the following steps:
1. Type an expression as the value of for a length adjustment. For example, d1*0.5.
2. Press ENTER. If the expression returns a positive value, then Creo Parametric prompts you for confirmation about whether you want to add the expression as a relation to the feature.
3. Click Yes to create the relation in the feature. This relation controls the extend value. The Length Adjustment options list becomes read-only and displays the value derived from the relation as a read-only value.
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After you have created the feature, you can modify the relation using the Relations dialog box that opens when you click Tools > Relations.
Trim at Reference—Trim a chain using a reference. Valid references consist of items that intersect the chain (surfaces, planes, curves, edges, axes, and so forth), or datum points or vertices that lie on the chain. This option activates the Trim at Reference collector enabling you to select a reference up to which the chain is trimmed. Notice that you can also use the Trim at Reference shortcut menu command from inside the graphics window to activate this collector.
Extend to Reference—Extends a chain using a reference. Valid references consist of items that intersect the chain (surfaces, planes, curves, edges, datum points, and so forth). This option activates the Extend to Reference collector enabling you to select a reference up to which the chain is extended. Notice that you can also use the Extend to Reference shortcut menu command from inside the graphics window to activate this collector.
8. To trim a closed-loop chain, click Excluded and select an edge or curve from the start point of the chain.
9. Click OK. Creo Parametric saves the changes, closes the Chain dialog box, and resumes the tool.
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Notice that as you modify a chain in the Chain dialog box, Creo Parametric dynamically displays the changes in the graphics window.
To clear references in the active collector, click Remove or Remove All on the shortcut menu that appears when you right-click in the collector. Alternatively, click Clear on the shortcut menu that appears when you right-click in the graphics window.
To easily locate references in the Chain dialog box, place your pointer over the reference in a collector. Creo Parametric dynamically highlights the reference on the model.