TRF6903 part symbol PCAD 2002 2

[SpaceTraveller]

Hi

I want to add the texas instruments RF IC TRF6903 to my schematic. on the TI website I found the CAD format in Axel, cadence, Orcad, mentor.

Can somebody tell me how I can add that part to my schematics.

Thanks,
ST

 

[zeitghost]

First thing we need to know is what schematic capture package you are using...

 

[SpaceTraveller]

OOps I forgot that!

PCAD 2002

 

[zeitghost]

Well, knowing nothing whatever of PCAD 2002, I can't really help other than saying that the part has to be added to a library (or libraries) of some sort...

This has the possibilities of being easy, like it used to be in dos ORCAD or very difficult, as it is in some other CAD packages I've used...

In the packages I've used (Orcad, Vutrax, CadStar), there's generally a schematic symbol library that the symbol is put in, and a footprint library that holds the physical representation corresponding to the schematic symbol.

Hope that helps, if only a little.

rgds
Zeit.

 

[SpaceTraveller]

Thanks Zeit.
I am trying to get in touch with the TI and see if they can provide the library for PCAD. THere is one other option I am left with, create my own symbol. I am working on that. In the latter case I cannot run simulation.

Zeit, Have you ever been in a position where the symbol was not readily available and you had to create one?

Thanks,
ST

 

[zeitghost]

Yup.

Generally causes me considerable distress.

There are few things I dislike more than creating new library symbols.

My classic was a symbol for the Z84c15fec10 microprocessor from Zilog where I managed to get the conversion from metric to imperial wrong... the footprint was about 80% of the required size... ooops.

All my schematic symbols in Orcad tend to be rectangular boxes, largely because that makes it very easy indeed.

rgds
Zeit.

 

[Noway2]

SpaceTraveller,

Creating new components in PCAD isn't too difficult. That is once you are familiar enough with PCAD and its clunky nature. I have found the PCAD libraries to be of very little help when it comes to the parts that I design my circuits with.

As for the procedure:

1 - you will need to create a new component in the library manager - and select the library that you wish to add the component to.

2 - this will bring up a dialog screen, were you need to enter the number of gates that the part will have, and the default reference designator.

3 - use the symbol browser and create a new symbol. You can start with the symbol wizard if you wish. The pertinant pieces of information are the pin name and pin designator. If you are unfamiliar with pin designators, they are the link between the pin name / number and the PCB pad number. For example, it is possible to have symbol pin 1, assigned pin a designator of 2 in the part symbol. Then have pad 5 asigned to pin designator 2 in the pattern editor. This means that symbol pin 1 will map to pad 5. When you are ready, validate the symbol to check for errors. You will need a reference point, referece designator, etc.

4 - Use the pattern editor to create a new pattern. You may (probably will) need to create new pad styles to match the component. You can use the information on the datasheet as a guideline. Note: In the pattern wizard, when it specifies the pattern width, it is refering to the pad - pad center spacing, which is not always specificed on a datasheet. Validate this piece too. Look to see if the manufacturer has a recommended land pattern and copy this if applicable.

5 - Once you have the symbol and pattern, select these files (that you hopefully just saved) on the main (new) component screen. Then go to the PINS view and verify that pin names, pin numbers, pad numbers, etc all match. You will likely have to fill in one or two extra columns, such as "pin equivalence"

Note, in the pattern editor, it is very helpfull to use the masure utility, with a very fine snap resolution (1 or .1 thousands) and verify that the pad spacing and sizing agrees with the part datasheet.

Also, the tutorials that come with PCAD, while not necessarilly intuitive, are a good way to get a handle on the process.

I am not certain what type of simulation you wish to perform. If it is using the signal integrity tool, you need to specfify the pin style (input output, power, etc) in the PINS View sheet.