Creating new Symbol
Using Resistors and Capacitors of Different Value
The .ptf file in the local_lib directory - local_lib.pft to be exact contains the different instances of the resistors and capacitors that can be placed in Schematics.
Here is a section of the local_lib.ptf file. The local_lib should have been included in your list of library as described in Library setup .
FILE_TYPE = MULTI_PHYS_TABLE;
PART 'RES'
:VALUE, TOL(OPT='5%'), RATED_POWER,PKG = VALUE, TOL , RATED_POWER, PART_NUMBER, JEDEC_TYPE, COST ;
100 , 5% , 1/8W ,1206 = 100 , 5% , 0.125 , CDN0005-01, 1206_T , .75
100 , 5% , 1/8W ,0805 = 100 , 5% , 0.125 , CDN0005-02, 0805_T , .62
1K , 5% , 1/8W ,1206 = 1K , 5% , 0.125 , CDN0005-01, 1206_T , .75
1K , 5% , 1/8W ,0805 = 1K , 5% , 0.125 , CDN0005-02, 0805_T , .62
END_PART
PART 'CAP'
:VALUE, TOL(OPT='5%'), VOLTAGE(OPT='25V'), MATERIAL(OPT='CERM') , PKG = VALUE , TOL, VOLTAGE, PART_NUMBER, JEDEC_TYPE, COST, ALT_SYMBOLS ;
82N , 5% , 25V , CERM , 0805 (82N) = 82N , 5%, 25V , CDN0004-01 , 0805_T , .13 , '(B:0805_B)'
0.1UF , 5% , 25V , CERM , 0805 (0.1UF) = 0.1UF , 5%, 25V , CDN0004-21 , 0805_T , .13 , '(B:0805_B)'
0.2UF , 3% , 25V , CERM , 0805 (0.2UF) = 0.2UF , 3%, 25V , CDN0004-22 , 0805_T , .13 , '(B:0805_B)'
0.4UF , 5% , 25V , CERM , 0805 (0.4UF) = 0.4UF , 5%, 25V , CDN0004-23 , 0805_T , .13 , '(B:0805_B)'
END_PART
PART 'XTALOSC'
CLASS = IC
:FREQ = FREQ, PART_NUMBER ,JEDEC_TYPE , ALT_SYMBOLS,COST;
42MHZ = 42MHZ, XTAL_42_DIP,OSC_DIP4 ,'(OSC_SMD4)',1.43
50MHZ = 50MHZ, XTAL_50_SMD,OSC50_SMD4 ,'(OSC_DIP4)',2.16
END_PART
PART '74F04'
CLASS = IC
:PACK_TYPE(OPT='SOIC'), MANUFACTURER(OPT='TOSHIBA') = JEDEC_TYPE, PART_NUMBER, COST, STATUS ;
SOIC , TOSHIBA = SOIC14 , CDN0000-44 , .89 , PREF
SOIC , TEXAS-INST = SOIC14 , CDN0000-74 , .93 , NONPREF
SOIC , NATIONAL-SEMI = SOIC14 , CDN0000-64 , .94 , NONPREF
DIP , TEXAS-INST = DIP14_3 , CDN0001-44 , 1.46 , NONPREF
FLAT , TEXAS-INST = PLCC20 , CDN0003-44 , .96 , PREF
END_PART
If you wish to add another resistor, of value, say 33K, you can add another line in PART 'RES' section as
PART 'RES'
:VALUE, TOL(OPT='5%'), RATED_POWER,PKG = VALUE, TOL , RATED_POWER, PART_NUMBER, JEDEC_TYPE, COST ;
100 , 5% , 1/8W ,1206 = 100 , 5% , 0.125 , CDN0005-01, 1206_T , .75
100 , 5% , 1/8W ,0805 = 100 , 5% , 0.125 , CDN0005-02, 0805_T , .62
1K , 5% , 1/8W ,1206 = 1K , 5% , 0.125 , CDN0005-01, 1206_T , .75
1K , 5% , 1/8W ,0805 = 1K , 5% , 0.125 , CDN0005-02, 0805_T , .62
33K , 5% , 1/8W ,0805 = 1K , 5% , 0.125 , CDN0ARBT-02, 0805_T , .62
The JEDC_TYPE defines the footprint for the component.
The same thing can be done for capacitors as well.
Using Part Table Editor
Although, the above procedure works, it may be a better idea to use the in built Part Table Editor to add new parts. Use Tools -> Part Table Editor and then navigate to the .ptf file in your library directory.The rest is easy to follow. Once you create or edit part, it will check for errors.