Fundamentals > User Interface Basics > Chains and Surface Sets > Chains > To Construct a Chain
  
To Construct a Chain
1. Select an edge or curve on your model to establish the anchor. Creo Parametric highlights the selected edge or curve.
2. Press the SHIFT key and move the pointer over to an adjacent segment. The preview of the one-by-one chain consisting of the anchor and the adjacent segment is displayed.
3. Holding down the SHIFT key, right-click and do one of the following actions:
Click Pick From List on the shortcut menu. The Pick From List dialog box opens which contains all the possible chains that you can construct using the anchor and the adjacent segment. Select the desired chain from the list. The preview of the chain is displayed in the graphics window. Click OK to accept the selected chain and close the Pick From List dialog box.
Click Next or Previous on the shortcut menu to preview the next or previous chain available for selection without opening the Pick From List dialog box. Click to accept the selected chain.
Right-click to query all possible chains associated with the anchor. Valid edges and curves for each possible chain are highlighted and aToolTipidentifies the chain type, for example Tangent, Surface Loop, or One-by-One. Note that the pointer must be near the selection and not over a handle to be able to query possible chains. If you are constructing a From-To chain, place the pointer over the edge or curve where the chain will terminate and right-click to query through the possible chains until you locate the From-To chain.
Click the highlighted item associated with the chain type that you want to create. Creo Parametric constructs the chain and highlights it.
 
* If you are working with a tool closed, the Selected Items area indicates the selection and the Selected Items dialog box contains the chain. If you construct a chain from inside a tool, the active collector contains the chain and the Chain label is displayed on the model.
4. If you are constructing a One-by-One chain, holding down the SHIFT key, click on the anchor again, and select additional edges or curves to include in the chain. Creo Parametric appends and highlights the chain. Alternatively, holding down the SHIFT key, move the pointer over to an adjacent segment. The one-by-one chain consisting of the anchor and the adjacent segment are pre-highlighted. Click to accept the one-by-one chain. Select other segments to add to the one-by-one chain.
5. If you want to construct additional chains during the same workflow, release SHIFT, hold down the CTRL key and click an edge or curve on your model to select an anchor for the new chain. Release CTRL repeat step 2 through step 5.
6. Open a feature tool or continue working in a tool to use the chain to create a feature.
 
You can remove an entire chain from the selection set by holding down the CTRLkey and clicking the chain to remove it.
After you close a tool, Creo Parametric restores the selection set that you constructed before opening the tool. You can continue to use your chains in other tools, without having to reconstruct them.
When you construct a Partial Loop chain, that is, a From-To chain using direct selection in the graphics window, Creo Parametric remembers the first selected edge or curve as the anchor reference and the second selection as the extent reference. If the extent reference is a one-sided edge and is the same as the anchor, then when you query this edge, Surface loop from to appears once in every query cycle. If the extent reference is a two-sided edge and is the same as the anchor, then when you query this edge, Surface loop from to appears twice in every query cycle.
You can use a continuous intent edge to construct a One-by-one chain.
To exclude a continuous intent edge or a composite curve located at the end of a chain, query the edge or curve and select it.