My Hobbies - Circad Course - Lesson 5
Schematic Components Making

Parabola

Barra Colore


In this lesson you'll create che schematic component called CN1. So, you'll be able to add the CONN1 component into the TUTOR1.SCH electric scheme. The component will be linked with MP5 pcb component, that is part of the standard library file PCB.LIB of Circad.

The component CONN1 must be created into a library containing schematic component, so isn't possible to use the COMP_PCB.LIB library file, in which are been stored the pcb component MIOTRAN. Then you must create a new library file containing schematic components with FW + "Schematic Files = Size A" + C:\Programmi\Circad98\Library\Comp_Sch.LIB .

To create the component you need to follow the same steps of the MIOTRAN component creation. In case of schematic component the elements (shape, pads, etc.) placing is not so critical like for pcb component. In fact, the pcb component shape must be equal to the real component, but the schematic component shape can be create as the user wish.

The component above is 300 x 600 mils; the pads are 200 mils far and they have a diameter of 60 mils, but you can create the component bigger or smaller, or with the pads more or less distant, or with a different shape.

First, place the component pads with PP. The pads must be placed into the Master layer (that is equivalent to the Pad Master layer seen for pcb components), using a 60 mils diameter, without hole ("Hole Size" = 0). Every pad placed must have a different name from the other ones, then insert the value 1, 2 or 3, due to the placed pad, into the "Pin Name" field.

In case of schematic component, every pad can be only of T0 type (square schematic pad) and cannot be modified.

Now place the component outdraw (the component perimeter) with PL. Select a 10 mils for the line thickness (but you can use the value you wish) and Symbols fot the layer.

Place the CN1 and &1 labels, respectively above and beside of the component (or in every place you like), using PT using, for example, a text dimension of 60 mils. The pin numbers can be placed, optionally, with the command PT, using a text dimension of 48 mils and Pin Numbers for the layer.

Now, with BI or BG select an area that include che component and the label &1, without the label CN1. To complete the elements selection, click in the center of one of the pads, e.g. the middle pad.

Then, use BB to make the component CN1 from the hilighted elements. Fills the form fields that will be showed with "Pattern" = CN1, "RefID" = CONN?. The fields "Type/value" and "Modifier" can be left blank.

Now, the component CN1 is ready to be used as component CONN1 of TUTOR1.SCH electric scheme. Then open the file TUTOR1.SCH, use SF to add the file COMP_SCH.LIB into the library file list where Circad will search for components. Place the component CONN1 with PC, using "Pattern" = CN1, "RefID" = CONN1. The fields "Type/value" and "Modifier" must be left blank.

In the "PCB Pattern" field enter MP5, that is the connector Molex - 5 ways, included in the Circad standard library file PCB.LIB. It's not a must that a schematic component must be linked to a pcb component with the same number of pins. In fact, Circad will try to link the schematic component pins with the relative pins of the pcb component.

If this will not happens, you'll have an error when you'll create the netlist of the electric circuit. The netlist is the the whole of the wirings between schematic components and the relative pcb components linked. If some pins of a pcb component will be unused, you'll obtain only a warning message.

To verify the pin number of a pcb component, you can use the command EP, over the pad analyzed. Also, it will be possible to modify the type, the dimension and the number of the pins of MP5, into the standard library file PCB.LIB, or into the file TUTOR1.PCB, that contains the printed circuit board of the electric scheme drawned in TUTOR1.SCH.

It will be possible to resize the pads, changing their shapes from square to round, or modifying their number, like swapping the pin 1 with the 4 and the pin 5 with the 2.

If you modify the pins parameters of the component MP5 placed into the library PCB.LIB you'll automatically modify only the components MP5 that from the time of the change will be used, for example with the command PC. The MP5 components already present in other files will be not changed. This because the link between schematic and pcb elements make a simple copy of the component you get from the various Circad library to your user file. This is true both for schematic and pcb components.

If you modify the pins parameters of the component MP5, placed in a single pcb user file, you'll change only the parameters of the component placed into the file.



1 - 2 - 3 - 4 - 5 - 6 - 7 - 8 - 9 - 10 - 11




Indice Index Storia History Curriculum Curriculum Pensieri Thoughts Cittą Cities Hobby Hobbies Link Links Novitą News
Scrivetemi Write me Guestbook!