My Hobbies - Circad Course - Lesson 2
Components Placing

Parabola




Now we will place the R1 component of the electric scheme. This will done using the PC option. In the Pattern field it is possible to directly specify the name of the components that we want to place. Circad will search the component into the library files indicated with the SF option, showed in the left bottom of the form. Then, to add or to remove lirary files you must use the option before.

The component is located in the DISCRETE.LIB library file, so select this file, then select the Resistors - Standard 1/4 Watt - Horizontal, identified by 'RS'. After the selection of the RS' component you will insert the value of the component (47 Kohm), and optionally the Modifier, that is a sub-type component, and the name of the relative component that will be used to make the pcb layout.

In this case to the R1 component it's been automatically assigned the pcb component called R400P70. The relationship between .SCH and .PCB components is already defined for the standard library Circad components, but this is not true for the newly created user components. For these components the link will be created by the user for every single schematic component.

The label R400P70 means Resistor with 400 mils far pads and 70 mils pads diameter. This is only a remember for the user, in fact if you specify R400P90 you don't obtain a 90 mils component pads, but only an error when the pcb creation, because there are no pcb component pattern (its name) equal to R400P90.

The component R400P70 is included in the THD.LIB standard library file contained in the /Library subdirectory. This library is defined in text mode, so isn't possible to see the pcb shape of the resistor. Then, we'll use the pcb component R400, included into the PCB.LIB standard library, that is the same as the R400P70 component.

To add a special caracter, like the ohm symbol, you must use the combination Alt + code, where the code is a value entered by the numeric keypad. In the table below you'll find the code to use to obtain the most common symbols. Use this mode to insert the symbols in the Windows forms. Else, to insert the symbols when you edit a text use the codes between parenthesis.

1/2 = 0189 (o Alt + 2)1/4 = 0188 (o Alt + 4) 3/4 = 0190 pigreek = 0182
micro = 0181 (o Alt + u) ohm = Alt + o +/- = 0177>> = 0187
<< = 0171 between = 0247 diameter = 0216 / 0248beta = 0223

To see the shape of R1 you must open, with the FO option, the libray file C:\Programmi\Circad'98\Library\Pcb.LIB, seeking the component R400, that you can see beside, with all the other pcb library components,associated with its relative .SCH component.

After you've entered the data, it will be possible to place the component into the selected position. When and after you place a component, you can move and rotate it again, using the options of the GRAB menu. The component can be deleted using the DC option.

Attention!!!
The Circad DOS version DOESN'T HAVE the Cancel or the Un-do function. So, every command (like deleting a component or moving a block) cannot be cancelled. The only way to go back is to close the file without saving the changes!!!



\/

After you've placed the component you'll be able to modify some parts of its. In fact, every element of a Circad file, is an object, also if it's linked to other objects. The label 47Kohm near R1 is joined with this component (if you move R1 the label will move with R1, but it does'n happens the contrary), but it's totally indipendent for its characteristics, like size, layer and rotation.

For example, use ET or EX or GT+R to modify the position or the appearance of the label mentioned above. It's not possible to modify the lines that draw the shape of R1, because it is a grouped component and it is not assumed maked by indipendent lines. In the Windows Circad version it's possible to modify component symbol line, but only for some components.

Now, in the same mode, you'll must place the components R2, D1 and Q1. You can use the library search method, or directly the pattern available in the table below. For Q1 you must specify MIOTRAN, a pcb component that doesn't exists in any Circad library file. In the next lessons we will create MIOTRAN, that is the shape of the pcb component of Q1, that is a BC547 transistor. The CONN1 component will be placed later... because it doesn't exists and, first, we must create it!

In an electric scheme it's normal to have more than one transistor, every of each represented, for example, with the shape of an NPN (the schematic pattern of Q1) transistor, but every component can be associated with a different kind of a pcb component. If you modify the pcb component shape, direclty into the library file in witch is contained, when you create the pcb layout, Circad will use the new modified shape.

Componente Pattern Ref. ID Type/Value Modifier PCB Pattern
R1
R2
D1
Q1
RS'
RS
LED
NPN
R1
R2
D1
Q1
47 Kohm
1 Kohm
LED
BC547
1/4 Watt
1/4 Watt
Nothing
Nothing
R400
R400
LED
MIOTRAN


Now you must place the power signal points. It's possible to place positive, negative or ground signal points. With the P+=+VCC option we'll place the two positive power signal points of the circuit. With PG you'll place the ground points. The +VCC label is only a conventional name of the positive signal, but you can name it in every (legal) mode you wish. The important thing is to call in the same mode all the signal that you wish to connect togheter.

The CONN1 wasn't placed, but you can place its power signal points, near the Q1 and R2 components, or you can place it later. Also the power signal points are objects and it can be moved, deleted, rotated, etcetera.


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!