My Hobbies - Circad Course - Lesson 4
Pcb Components Making

Parabola

Barra Colore


Now you'll create the pcb component MIOTRAN, that is the up view shape of the component Q1, as seen in the TUTOR1.SCH schematic file.

The component will be made into a library file containing pcb components. A library is a file with a schematic or PCB template, but it's saved with the .LIB extension and stored into the \Library subdirectory. The library must have a schematic template if it contains the electric symbol of components for .SCH file, or it must have a pcb template if it contains the pcb shape - that is the "real" shape - of electronic components for .PCB files.

Then, create a library file with FW "PCB Files = Size A" + C:\Programmi\Circad98\Library\Comp_Pcb.LIB.

To create the component you'll follow the next steps, first placing the crosshair cursor in any point of the screen.



A - Place the Emitter pin pad with PP. Then, Circad will show a form in which you'll must specify the pad name "Pin name" = E, the pad external diameter "Pad size" = 70 and the hole size diameter "Hole size" = 30. The "Layer" and the pad type "Pad type code" are preset by Circad, but if you need a square pin or a pin placed into another layer, you'll must only change the default values. For example, a round pcb pad have a T1 pad type, and a square pad have a T2 type.

The pads can be placed in every layer, but if they are component pad must be placed into the right layer, that is the Pad Master layer.

B - In the same mode place the Collector pin pad, using the value C for the "Pin Name", then insert the same values of the Emitter form. Circad, usually remember the values inserted into the various forms, so probably you'll found the correct values already presetted. The pad must be placed at 150 mils, horizontally, from the Emitter pad.

C - Now you must place the Base pin pad, using the value B for the "Pin Name", then insert one more time the same values of the Emitter form. The pad must be placed half between the Emitter and the Collector pads, vertically moved by 75 mils.

D - It's time to draw the real shape of the component, reminding that the shape of the component is intended up viewed, or viewed from the component side of the pcb. Using a snap grid of 25 mils you'll be able to copy the shape in the imagine beside, but you'll can draw a similar shape. This because the draw of the shape of the components is never analyzed by Circad. It's indispensable that the component shape will be the same of the real component, to avoid the risk of real components that don't fit into the pcb... because they are been drawned too small!

With PL and "Layer name" = Top Silk and "Line thickness" = 10 mils, you'll be able to draw the component shape. Using the layer above the component will have a shape into the component side of the pcb. If you need the shape into the solder side use the "Bottom Silk" layer, also placing the one on the top of the other. To view the one or the other, use SL to activate and/or disable the the right layers.

E, F, G - To place the pad names, move the mouse near the pad, then use the PT command, with "Layer name" = Top Silk, "Text Size" = 30 mils, "Rotation" = 0°, then writing the pin name. The pin shape name can be different from the real pin name, used during the placing phase of the pad. So, you can specify "E" or "EMIT", etc.

H, I - Following the same previous step instructions, place the text "&1" and "&2", respectively above and below the component shape, reminding that the "Text size" and "Rotation" must be equal to 48 mils and for the first text and 18 mils and 315° for the second one. This special text indicate to Circad that we are placing fields related to the component. This value will be not static, but will change dinamically linked with the "Ref ID" field (for &1) and to the "Type/value" field (for &2) of the component. The default value of this fields, that will be inserted later, during the elements grouping, are these that you can see during the component placing phase.

J - The last step, optionally but suggested, you have to do is to place a text to fast identify the pcb name of the component shape. Following the same instructions for the E step, now you must place the text MIOTRAN above the component shape, using "Text size" = 48 mils.

Now it occours to select the shape elements area that will be grouped togheter into the MIOTRAN pcb component. Use BG to define a rectangular block, that is an area outside the elements placed before, clicking near the point indicated by the arrow in the figure beside, without selecting the MIOTRAN label. If you select the label into the hilighted area, every time you'll use this component, it will came into the pcb with its name. The command BG also ask to you to specify a reference point every time you select an area. Then click in the center of the collector pad. This will be the the reference point when the component will be placed, moved, resized, etc. If you make some mistake during the block definition, use BE to cancel it.

Now use BB to create the component from the hilighted area. Fill the form field that will be displayed, exactly than below, speficing "Pattern" = MIOTRAN, "Ref ID" = Q?, "Type/value" = BC?. So the program will group all the selected elements, considering it only one component called MIOTRAN. The "PCB Pattern" field must be left blank, because it's used to assign the default pcb footprint, but only for schematic component.

After you've filled the previous form fields, the labels &1 and &2 will be changed in Q? and BC?. Now the MIOTRAN component is now maded and it can be used into the pcb as a shape of any component of an electric scheme that have three pads named E, B, C, like the NPN transistor BC 547.

After the component creation will be possibile to modify the component shape (only the textual part) and also other component parameters.

To dissolve the component and to have the before created single elements use GC + EK. Now you can re-create the MIOTRAN component, following the previous steps.



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!