Parts, Sheet Metal, Solid Edge, Tips
Creating and Using The (Ordered) Feature Library
Purpose: The aim of this tutorial is to learn how to create and re-use a feature from the Feature Library. In this case we shall create a pair of positioned holes in a sheet metal part, although these could be created in either a sheet metal or part file.
Create a new sheet metal file and ensure that you are in the Ordered mode.
- Using the Tab command, create a 300mm x 100mm rectangle by centre, centred about the reference planes. Click the Close Sketch button and project the Tab down, with a thickness of 1mm.
- Click the Hole Feature and select the top face of the tab.
- Set the Hole parameters to a 10mm simple hole, set to go through next.
- Place 2 holes (making sure that the 2 holes have a horizontal relationship between them), positioning the first 20 mm from the right end and the second that is 40 mm from the first (as shown).
- Place the dimensions as shown, ensuring the dimensions are locked. Having the dimensions locked ensures that the dimensions are linked to the feature in the library and are retrieved when the feature is placed.
- Close the sketch and project the holes down through the part.
- Click on the “Hole 1” feature in the pathfinder.
- Click on the Feature Library tab and set the directory to where you would like to save the feature to. Click the Add Entry button (as shown). The feature(s) needs to be already selected for the “Add Entry” to become active.
- The Feature Set Information box displays what will be stored with Feature in the Library.
- When you close the Information dialog box, Solid Edge will prompt for a file name, so enter a name with some meaning and click Save. The feature will be labelled with a .par extension, but isnot a standard part feature.
- To place the feature in a new part/sheet metal part, open the Feature Library tab and drag the feature into the document.
- The Feature Set Information dialog box is re-displayed to show what is required to place the feature. As this feature was created as a Ordered feature, you will need to be in the ordered mode to place it.
- The first step is to select the reference plane to place the holes into. In this case we will select a flange on the side of the part. The holes were created with the through next option, so the thickness of the flange is immaterial.
- There were 2 dimensions on the saved feature, one dimensioned between the holes and the other dimensioned to an edge. The dimension between the holes is fixed, but the next step is to define which edge we should attach the edge dimension to.
- Select the edge to complete the placement of the feature. Should you need to, you can select the direct edit option for the inserted hole feature and adjust the dimensions.
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