Fundamentals > Creo Parametric User Interface > The Analysis Tab > Analyzing Model Properties > To Calculate Clearance Between Two Entities
  
To Calculate Clearance Between Two Entities
1. Select any two curves, edges, datum points, surfaces, pipe segments in Assembly mode, cable segments in Assembly mode, cables in Assembly mode, parts in Assembly mode, or components in Assembly mode.
2. On the Analysis tab, click the arrow next to Global Interference and then click . The Pairs Clearance dialog box opens. Quick is the default analysis type.
3. Click OK to complete the analysis or Cancel to cancel the analysis.  Alternatively, click Repeat to start a new analysis.
4. Optionally, to save or create an analysis feature, perform the following steps:
a. Click the Analysis tab if it is not selected by default.
b. Select the desired analysis types from the list at the bottom of the Pairs Clearance dialog box.
c. Select Saved to save the analysis with the model, and dynamically update the analysis while modeling or select Feature to create advanced features.
d. If required, rename the analysis in the box adjacent to the list.
e. Click the Feature tab to create or change feature options of the current analysis, if required. You can access the feature options such as parameters or datum features only when you select a feature type of analysis.
5. Optionally, to customize or edit your analysis, perform the following steps:
a. Click in the From collector and select the required entity. The name of the selected entity is displayed in the From collector. If the From entity is a surface, Whole surface and Near pick options are activated to select the Geometry from which you want to calculate the clearance . Whole surface is selected by default. If you click Near pick, you can select only a surface in the To collector.
 
* In the Assembly and Drawing mode, you can also select quilts or facets of the selected part, subassembly, surface, or cable in the From and To collectors to compute the clearance.
b. Click in the To collector and select the required entity. The name of the selected entity is displayed in the To collector.
6. Select a reference plane, coordinate system, surface, axis, edge, curve, or datum plane in the Projection Reference collector. The projected clearance and actual clearance are displayed in the result area at the bottom of the Pairs Clearance dialog box.
7. If required, click to view the projected clearance and actual clearance report in the Information Window.
 
* If you select a coordinate system to project the direction in the Pairs Clearance dialog box, you can select the required coordinate system in the Creo Parametric graphics window. Projected clearance is displayed for the x-, y-, and z- directions.
8. Click Preview to compute the analysis. The clearance between the two entities is displayed in the result area at the bottom of the Pairs Clearance dialog box.