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.