Blog

Tutorials, news, snippets, and other various musings about the electrical engineering industry.

Capture Walk-through 2: Creating Parts

This tutorial demonstrates several ways you can create and add parts to a Capture library in version 17.4 (2021). After you complete this tutorial, you will be able to: 
 

  • Copy library parts and paste them into a new design library 
  • Rename and edit a library part 
  • Create a new part and add it to your design library 
     

To follow the instructions presented in this tutorial, continue using the design you completed in Capture Walk-through 1 or use the included design file, CAPTURE TUTORIAL 2_CREATING PARTS.DSN. 



 

  • Select File > Open > Library from the menu.  




 

  • Use the following path to access the default libraries provided in Capture: C:\Cadence\SPB_17.4\tools\capture\library 


  • Open the CAPSYM.OLB library. 


  • Note: Click on the arrow located in the right of the library, to change the view of the window: docked, floating or a tabbed document. 



 

  • Select Ground_Power and Titleblock3 in the capsym.olb library. 

 

Note: To select multiple items, hold down the CTRL on the keyboard and select the desired items. 

  • Use CTRL+C on the keyboard to copy.



 

  • In the Capture Tutorial project hierarchy, right click on the Capture Tutorial library and select Paste.  




 

  • Right click on GND_POWER and select Rename. Rename the part to GND. 
  • Right click on Titleblock3 and select Rename. Rename the part to TitleBlock. 



 

  • Right click on the Capture Tutorial library and select New Part.  



 

Enter the following information: 

  • Name: USB-MicroB 
  • Part Reference Prefix: 
  • PCB Footprint: USB-MicroB 
     

Note: Use TAB on the keyboard to quickly go to the next field. 
 

  • Click OK




 

  • Click the boundary part and drag the vertex to resize the boundary box. 
  • Select Place > Rectangle from the menu.  
  • Click and drag to draw the rectangle.  
  • Right click and select End Mode (ESC)
  • Select Place > Pin from the menu. 



 

Enter the pin properties below in the Place Pin dialog window: 

  • Name: GND 
  • Number: GND 
  • Shape: Short 
  • Type: Input 
  • Click OK
  • Click a location on the part boundary to place the pin. 
  • Use Shift+G on the keyboard to re-open the Place Pin window. Enter the values for the next pin. 
  • Continue placing pins using the pin properties below.   



 

Note: When the pin ends in a number the next pin placed will be sequential. You can continue to click and place MT1 to MT4 and P_1 to P_2 without editing properties between pins. 
 

  • Right Click and select End Mode when finished (ESC)



 

  • In the Property Sheet, de-select the Pin Name Visible check box. 
  • Select the Value text. Right click and select Rotate. 
  • Click and drag the text to a new location. 
  • Double click the text. 
  • Change the value to USB-B and Enter. 




 

  • Right click the part tab. Select Save and Close
     

Note: A part can be viewed and edited by double clicking the name in the library. In the Property Sheet, select Edit Pins to edit all the pins in the part. 

Software: