Edit component

Overview on component drawing (showing the principle)
Create a new component (best practise)

Has anyone else drawn my part already?

Before you start drawing, have a look at COMPONIVERSE, a place to share TARGET parts. Maybe a friend out there has already drawn your part and shares it. Alternatively have a look at each the component portal Ultra Librarian or Samacsys to download CAD data of your desired part in TARGET format.

If you want to draw a component completely new, please start with the package (footprint pattern).

You may use the Package Generator which at the same time provides a 3D model.

As an alternative you may use the Package assistant for devices having a huge amount of leads. You may also draw the component freehand. This article explains in detailed steps, how to create Component Packages, Schematic Symbols, and Reference Symbols.
For 3D models please have a look here: 3D or see the Package Generator.

TARGET 3001! understands a component as the dualism of a component package and one or more schematic symbols. It is recommended to draw the component package first and save it to the database. The reason for this is when you draw a schematic symbol and want to save it to the database, you get asked to assign a package to it which later appears as a "package proposal". Therefore, it is good to have the desired package already available. Later, when the import of an appropriate component package to a layout is required, the above package proposal is optional. That means you can use it but you also can leave it and use a different one, a "free package".

It is recommended that TARGET 3001 users get familiar with the above feature by opening an empty project to try a few examples, and "play around" with this feature. The grid-size should be set 0.635mm = 25mil. It is recommended to have the pin-to-pin distance in the schematic 2.54mm = 100mil = 0.1in (= 4 grid steps). Maybe the quickest way of getting results is to modify existing footprints or symbols. So let's start with this topic.

How to modify an existing component

Let's say you intend to use one of the TARGET 3001! SMD resistors with package 0402 but wish to give it different values. You would just make a copy of it and furnish it with your desired values. This is the way to proceed:

Image1: Start with the "Parametrical search" in the component browser

Image2: The one you copy necessarily needn't be a green one. Green means: "All entered parameters match". Regarding mousekeys please follow the link.

Image3: Yes, you want to copy the package in order to make it a USER package

Image4: Within your user copy you now do your settings and amendments.

Image5: Go through the tabs to do all your custom entries. Done.

How to modify an existing package

TARGET 3001! allows to modify any package (footprint pattern) separately and save it again as a new (USER-) component. Please press [F2] to start the Component Database browser. Select the tab "Package" (1). Enter "ssop" (2). Right-click M2 on a package name in the list opens a context menu (3). Select "Edit package drawing (PCB Layout)" (4).

Image: Edit a ssop28

Change the component using the drawing functions. Select all, hover the mouse over the old handle cross. Press key [x]. Change the name or other properties. Press OK. The component is saved as a "USER" component now with a black flag. Assure to have "My components" checked with a checkmark on right top of the dialog.

To use the drawing functions while editing an existing component watch this, it is a little more detailed: Guess you are in a design flow and recognize that the Dil_10 you are searching for is missing. Your idea is to modify the Dil_8 from the database to a Dil_10.

1. Open a new "PCB without schematic". By this means the component browser only shows the packages which contain the footprints. In case you have opened a "PCB with schematic" you first have to switch over to the layout view and select "free package" from the list of package proposals. Don't worry - this works too. The following instructions refer to the situation of a "PCB without schematic".

2. Import DIL_8 from the database into the PCB canvas.

After pressing Edit component you see something similar to the following picture. Choose the format filling scaling factor by key [F7] for a more convenient view.:

3. Now highlight Pad N° 5 by M1 for copying it by [Ctrl]+[c]. (You might copy any other pad...)

4. Now you have it in your clipboard. Now press [Ctrl]+[v] for pasting it. It's pictogram is fixed to the cursor:

Move it to the left starting from it's initial position to figure out the pitch (distance between the drillings) defined by grid steps. If it does not mantch, please try to set the grid accordingly. Take care for having a grid-move in one step units.

In our example we have a grid of 4 steps. That is the distance we paste the pad to the canvas:

and

Do the same in the bottom row:

and

5: Now we have to renumber the pads. Within the lower row the numbering is ok, but in the upper row adjustments have to be made. We double click M11 the upper right pad and have to change the pad number as follows:

Result:

Do the same with the remaining pads of the upper row so that they look that way at the end:

6: now we have to shift the outline of the package. We touch and hold M1H and drag it to shape. You also can hold it and use the arrow keys of the keyboard in order to jump by grid.

and

Confirm the warning message

("Yes, you really want to tear it to pieces...")

and get:

7. Double click the handle cross (at pad N° 1) and change the value from DIL8

to Dil10. What you get is:

8. Highlight the new package (drawings, solder pads and names must be marked completely) with the mouse.

9. Place the cursor on the spot, where the handle-cross should appear. Attention: It is not necessary to delete the old handle, because TARGET overwrites it automatically.

10. Press the [x] key.

11. The "Export Package" dialog appears. Give it a name and a component type within a component group. For versions older than V14 you would select a library to put it in.

12. Select OK (Return key). Done.

If you intend to assign a symbol to it, please use button "Assign a symbol" in the step 7 dialog.

How to modify an existing symbol

TARGET 3001! allows to modify existing components and export them back to the data base as new components.

Example: You want to change the existing schematic symbol for the smd inductivity SM-B5 into a magnetic shielded smd inductivity SMs35.

1. Open a new project with an empty schematic page.

2. Press function key "F2" and search for component "SM-B5". Now press the "Edit symbol" button. You get asked to create a user copy of it. Confirm this dialog and get the part to the schematic page.

Image: The F2- browser allows edition of a symbol. You also might klick right (M2) on the image of the symbol, bottom left in the dialog.

3. For better editing, please select the format filling scale factor with the [F7] key.

4. Now do all the necessary changes with the help of the drawing functions. Take care to have this switch constellation in the sidebar:

You can of course add new pins, add text or do whichever changes needed. If you want to delete an element, place the cursor in pointer mode upon an element, press [s] for "select" as often until the element in question is flashing. Now press [Del]. M11 upon the element in most cases does the same.

5. Highlight the new symbol (drawings, pins and names must be marked completely!), by dragging M1H in "pointer-mode" a highlighting square over the component.

6. Place the cursor on the spot where the handle should appear (it is recommended to place the cursor on the former location of the handle). Attention: It is not necessary to delete the old handle, because TARGET overwrites it automatically.

7. Press the [y] key for placing the handle.

8. Press the [x] key to export the component.

9. Enter all necessary information in the "Export Symbol" dialog.

It is important to choose the right package proposal for your component in the center bottom of the dialog.

Note also: Labelling of an existing component with !COMPONENT, !VALUE or !SYMBOL is not necessary, the existing names can be omitted. Changes and a new labelling are of course possible.

How to draw a package

Before you start drawing yourself, consider whether the package type couldn't be created using the Package Generator. The advantage is that autamatically a 3D model is provided.

You can easily create packages yourself. Say the LTC1392 IC from Linear Technology would not be part of the database. To create this component use the components original datasheet. It can be obtained from the Linear Technologies homepage at http://cds.linear.com/docs/en/datasheet/1392f.pdf

Package outline

Sketch of a DIP package according to the datasheet measurements of the package, dimension in inches (millimeters):

Sketch of an SO package according to the datasheet measurements of the package, dimension in inches (millimeters):

Lets start with the N8DIP package. For a convenient work with this article it might be good to have these two above images printed on paper besides you.

1. Open a new project "PCB with schematic" and switch to the empty PCB page and select menu View/Toolbars/Toolbar "Edit component" visible to get the toolbar to the left.

2. Select a suitable grid size. The pitch (= the distance between the centre of two adjacent pins) is 2.54 mm a grid of 0,635 mm (a quarter of the pitch) would be suitable. It is 1/40 of an inch. TARGET 3001! separates decimals by a comma, not a period. Set the above grid unit here: and here: Use the same dialog in order to display only every second grid mark. See dialog:

Window grid dialog

For the package outline a grid of 0,1mm is suitable. That means we have inch-sizes in mind but we set the scale metric, in millimeters (mm).

3. Draw the component outline on layer 21. Clicking the right mouse key on the layer number 21 activates this layer for drawing.

Layer number 21 underlain in gray indicates it being currently ready for drawing on.

After you have chosen the drawing tool the leftmost layer icon within the main toolbar (top egde of screen) indicates that drawing layer 21 is currently active.

4. Start by drawing an outline of the package. This is done with an "Open rectangle" from the drawing functions. Here the word "open" means "not filled", the opposite of "solid". Use icons and

Place a rectangle of approximately the same measurement as the package over the origin of the drawing. The exact coordinates of each line of this rectangle will now be entered.

You need to decide if you want to use inch (inch, ") or metric (mm) dimensions. We recommend metric scale in mm. Set the scale in the grid dialog. At any time you can switch the units using the function key [F4]. Set the dimensions of the rectangle within the tolerances according to the value table. For the body we recommend to take the larger values to be on the safe side when assembling the board later. The pitch we set exact without tolerances.

The coordinates in the status bar show the position of your cursor. Keyboard functional key [F4] toggles the units. The image below shows the cursor position in inch at 0,03937|0,06299 ". [F4] toggles to 0,533400|0,546100 mm.

The package shall be constructed, centered around the point of origin. So we start drawing a rectangle of any shape to any place:

"How to get my square to size quickest?"

We can see from the datasheet that the width of the package is 10,16 mm and the height is 6,85 mm. Double click a line of the rectangle in order to open a dialog for edition. Set "Position X" and "Position Y" to 0|0 and tick the box Center. Now just enter the measurements for Width and Height and say OK.

5. An outline of the package with the exact measurements has now been constructed, centred about the point of origin of the drawing. Now, in order to place a notch (mark) on the left vertical line, we select the left vertical line. This will cause little "catchboxes" to appear at the ends of the line and in the middle. Now press M2 upon the middle box and add two vertices. Vertex means another "bending point", represented by another black catchboxes created within the line. Again press M2' at the middle segment and convert it to an arc. Now set a little notch. Also a little circular mark can be set to indicate where Pad 1 shall be placed later. Or a line can be drawn or whatever...

Pads

Wired

6. The next step is to place the pads. The N8 PDIP package has solder pads with plated through holes (PTH) and a copper collar (ring) on both copper layers; which is the way a standard pad would appear taken away the FR4 substrate:

Now select the "place pad" option in the drawing tool:

The shape of the cursor will now change to:

Press the [o] key for options to set the dimensions of the pads being imported. Import them rotated by 90° if wider than high.

The settings for pad height and width as well as for the drillhole are defined by the datasheet, as shown at item (1) and (2) below.

Pads for wired packages are defined on layer 100, "All copper layers", because the galvanized drilling runs through all copper layers. If you choose a pad default from the selection of the drawing tool those settings are predefined. Pads for SMD packages are to be modified in the above dialog a bit: Layer = 16 ("Copper top"), Drill hole = 0mm, Form = rectangle.

Let us now examine the lead dimensions to define pad dimensions as well as the drillhole diameter. We enter 0,8mm as drillhole diameter (compare at 2, maximum value is 0,533mm so with 0,8mm we're OK). Pad height and width we enter 1,7mm for each (compare at 1, maximum value is 1,651mm so with 1,7mm we're OK).

The next step is to place the soldering pads. Set the grid to a quarter of the pitch (2,54mm : 4 = 0,635mm), click the pad icon to the left and start from the center of the body's base line.

Use the arrow keys of your keyboard and go 6 steps to the left to start with Pad number one. Place it by using keyboard key [1]. Go 4 steps right and press key [1] again in order to place pad number two and so on.

Still use the arrow keys for continuing with the upper row.

To set the y-coordinate, please highlight the complete lower row and press key [e] for edit. In the flashing dialog change only the y-coordinate to 8,255/2 = 4,1275mm, negative. Do the same with the upper row but change only the y-value to 4,1275 positive.

Doubleclick pad # 1 and give it a square form with a corner radius for identification when populating/soldering:

Place a variable component name (will be filled in by the symbol which uses this package) and a variable component value before you click the save icon. Now hover the mouse to the origin in order to place the handle cross there and click. Now you can save the package using an appropriate name.

SMD

For the creation of pads for a SMD package please act similarly. Only the options of the soldering pads have to be adjusted differently:

• The shape of the pads is rectangular with slightly rounded corners (rounded 20% is well. It means: The rounding radius is 20% the length of the shorter side of the pad)
• The drill hole has to be zero (= 0) because there is no drilling
• The copper layer has to be set from 100 to 16 (copper top) or 2 (copper bottom)
  

The pad dimensions (the landmarks) we draw according to the data sheet. Those are always a bit bigger than the pure leads of the housing.

We from TARGET 3001! draw the pads of an SMD device by default on layer 16 (copper top). So we have defined the mounting of our SMD package upon the copper top layer (the assembling layer). In case you wish to assemble the smd-component on the copper bottom layer (the soldering layer), please use the function "mirror" in the layout later. By this means it is flipped from the copper top layer to the copper bottom layer. Shall a SMD device be assembled on the bottom layer in general so please assign the soldering pads to layer 2 (copper bottom) in the following dialog. For the outline of the package use layer 7 (position bottom). Such an SMD component meant for bottom assembly can be flipped to the upper side later also by mirroring it. When drawing the component please have a cereful look at the drawing view-logic according to the data sheet. Many data sheets show SMD packages in "bottom view".

Settings for a smd-pad

Question:
"I am designing a two layer board with Texas Instruments TAS5704 chip (S-PQFP-G64 package) which requires thermal pad connected with vias:

Is there a way to design the package for this chip so that thermal pad is automatically generated?"

Answer:
First draw a normal SMD package as shown above. The center thermal exposure area create in the same way as a single SMD pad:
- use one SMD pad in square shape like determined by the datasheet
- place as much vias as you need in the inner area by using the full stop key [.]
- move them into position
- connect them to the plane by using tracks (= you must connect them by copper track, only the copper pad is not enough)
- now save the package to the database as usual
- Later when you have imported the package to the layout,
- highlight the inner pads/vias and double click them to open the "Change Vias" dialog:

- use the function "No aura for these layers"
- define the layer on which the aura shall be 0. (maybe 2=copper bottom, maybe 16=copper top)
- set the aura of the tracks to zero (= connect the tracks to the plane)
- give a signal name to the tracks, to the vias and to the plane (as long as this step is not yet managed by the schematic connection)

Save Package

After you have completed construction of the component package, catch it completely (drawing, solder pads and texts) with the mouse M1H.
Place the cursor on the spot where the handle cross should appear (on solder pad # 1 for example).
Press the [x] key (collecting the package with [y] as shown in the schematic is not necessary).
The "Export Package" dialog now appears.
Select the appropriate package type or create one by typing a new one to the line.
Enter a name for the package.
If a manufacturer is known, please select from the list or type in a new one. Otherwise leave it "not clear".
Click OK and the part vanishes from the canvas to the database.

The "Change package" dialog

The "Change package" dialog opens

• on double click upon the handle cross of a package
• on single click upon the handle cross of a package and pressing the keyboard key [e] for edit. Tick box for package and press OK.

The "Change package dialog"

The dialog: "Change package"

Position defines the coordinates of the handle cross of the package. X- and Y-value can be changed on one strike or only the X-value or only the Y-value, see drop down box. The package will be blocked against any movement if box is ticked.

The line Component contains name and value of the highlighted package. In this line no adjustments can be made. Only in the lines Prefix, Number # and Value. Prefix and number represent the name of a component.

The six buttons mean:
Variants - the maintenance of assembly variants (alternatives of assembly within the same project)
Properties - The list of properties of a component
Hide/Show name - Hide or show the component name (not the package name).
Hide/Show value - Hide or show the component value.
Note regarding earlier versions: Component name and -value can be faded in/out separately in the layout. Fading out by deleting from the layout. Fading in by: Highlighting the package in the layout, hovering the cursor to a place where name/value shall start. Starting the Text mode by pressing the ["] key. In the text dialog selecting Function "Component name" or "Component value".
Edit 3D model - self explanatory
Internal connection - Connections having internal load capacity can be derived from the schematic.
A Rotation of a package by degrees would not be defined within this dialog. Preferably it would be done using [Shift]+[t]. The entry here only shows a rotation which had been effected earlier.
The same with the entry Flipped (= from below) - it is only for announcing whether a part is assembled from the bottom side (box is ticked). No manipulation here - better done in menu: "Edit/Mirror"
The line Layer defines the layer on which the outline image of the package for position print appears. Normally it is layer 21, Position top. But also layer 7, Position bottom, is possible or any other reasonable layer of your choice.
Tick at Omit 3D display effects exactly this: No display of this package in the 3D view of the board.

How to draw a symbol

Ein TIPP vorweg...

Wenn Sie mit einem neuen Bauteil beginnen, erstellen Sie immer zuerst das Gehäuse (Lötfüßchenmuster) und dann das Symbol (Schaltplanzeichen), es sei denn, Sie benötigen kein Gehäuse, etwa beim Zeichnen von Symbolen für Stromlaufpläne in der Elektrotechnik. Beim Abspeichern des erstellten Symbols werden Sie nämlich gefragt, welches Gehäuse Sie dem Symbol als Gehäusevorschlag beifügen wollen. Wenn Sie noch kein passendes Gehäuse verfügbar hätten, müssten Sie das Symbol erstmal zwischenlagern, dann das Gehäuse erstellen, dann das Symbol wieder aufrufen, um ihm danach das Gehäuse als Vorschlag beizufügen. Dann erst könnten Sie das Bauteil in der Datenbank sinnvoll speichern. Besser ist es also, das Gehäuse schon verfügbar zu haben, um es einem Symbol bei dessen Erstellung zuweisen zu können.

LTC1392 - Das Datenblatt

Angenommen das Bauteil LTC1392 der Fa. Linear Technology fänden Sie nicht in der mitgelieferten Bauteildatenbank. Um das Bauteil zu erstellen, benutzen Sie als Vorlage das orig. Datenblatt dieses Bauteiles. Die für uns interessanten Inhalte stellen sich wie folgt dar:

Eine typische Anwendung im Schaltplan:

none

Draufsicht Gehäuse mit Pinbelegung:

none

Beschreibung der Pin Funktionen gemäß Datenblatt:

none

Wie zeichnet man das in TARGET 3001!?

Wählen Sie im Schaltplanmenü "Bauteile" die Option Neues Bauteil erstellen. Es öffnet sich der "Gehäusechecker" zur Auswahl des passendes Gehäuses. Es gilt: Erst das Gehäuse verfügbar machen!

noneBild: Der Gehäusechecker. Wählen Sie ein Gehäuse.

Wenn Sie die grüne Fläche klicken, öffnet sich links die Toolbar "Bauteil bearbeiten". Klicken Sie zunächst auf den Zauberstab um zu prüfen, ob eventuell ein Symbolassistent geeignet wäre:

noneBild: Der Zauberstab. Assistent geeignet?

Am einfachsten wäre es, ein generisches Symbol zu verwenden oder ein bereits vorhandenes abzuwandeln. Sehr schnell erstellt man ein Symbol mit dem Symbol-Generator. Wenn keine der genannten Funktionen hilft, zeichnen Sie das Symbol von Hand.

Ein Rechteck zeichnen|noneBild: Ein Rechteck aufziehen

Als Symbolkörper ziehen Sie ein Rechteck auf und konfigurieren es ggf. mit Doppelklick darauf. Das Datenblatt gibt keine Hinweise über die Abmessungen des Symbolkörpers. Zeichnen Sie also nach Ihren eigenen Maßgaben.

Anschlusspins platzieren|noneBild: Anschlusspins setzen. Doppelklick auf ein Pin öffnet den Dialog.

Setzen Sie alle Anschlusspins mit Mausklick aufeinanderfolgend zunächst neben den Symbolkörper. Die Nummerierung geschieht automatisch. Mit Doppelklick auf jedes einzelne Pin stellen Sie dessen Funktion ein. Dies geschieht im Dialog "Anschlüsse ändern". Laut Datenblatt ist Pin 1 ein "Digital Input", also stellen wir seine Funktion auf Eingang(IN).

Pin Namen vergeben|noneBild: Jedem Pin einen Namen geben

Der Knopf "Pin Name bearbeiten" erlaubt die Vergabe eines sinnvollen Namens für den Anschluss. Gut ist es, sich am Datenblatt zu orientieren. Wir benennen Pin 1 alos "D IN". So machen wir es mit allen Amschlusspins: Jedes einzeln doppelklicken und den Dialog "Anschlüsse ändern" bearbeiten. Gegebenenfalls müssen im Dialog die Checkboxen "Inverter", "Takt" und "Ist Referenz-Anschluss" bedient werden. Nachdem alle Pins konfiguriert sind, erhalten wir folgendes Bild:

noneBild: Anschlusspins sind konfiguriert

Den Pfeil bei CLK, Clock, erhalten Sie indem Sie im Dialog "Anschlüsse ändern" den Haken bei "Takt" setzen. Den Kringel bei dem Inverter-Pin erhalten Sie, wenn Sie im Dialog "Anschlüsse ändern" den Haken bei "Inverter" setzen. Den Pin-Namen CS des invertierten Pins versehen Sie mit einem Überstrich, indem Sie im Dialog "Anschlüsse ändern" den Knopf "Pin-Name bearbeiten" drücken. In der Textzeile versehen Sie die Buchstaben CS mit einem senkrechten Vor- und Hinterstrich, also so: |CS| Diesen senkrechten Strich (Pipe) erhalten Sie durch [AltGr]+ [<]. Regel: Alles was im Namen überstrichen sein soll, muss sich zwischen zwei senkrechten Strichen befinden.

Die Anschlusspins verteilen

Verschieben Sie jeden Anschlusspin mit gehaltener Maustaste M1H an eine geeignete Stelle des Symbols. Ggf. müssen Sie ihn während des Verschiebens mit Klick auf die rechte Maustaste M2 drehen. Man kann auch einen Pin im nachhinein drehen. Markieren sie ihn und drücken Sie die Taste [d]. Dreh-Achse ist die Cursorposition! Wenn Sie den Cursor zu weit weg bewegen, drehen Sie den Pin ggf. aus dem Bild und sie fragen sich "Wo ist er?". Wenn dies geschieht hilft auszoomen.

none


Hinweis: Die Versorgungsanschlüsse (Power), Pin 5=GND und Pin 8=VCC, können ins Symbol mit hinein genommen werden, können aber auch separat behandelt werden. Im letzteren Fall werden sie später auch separat in den Schaltplan herein geholt und abseits vom Hauptsymbol angeschlossen. Dies dient der Übersichtlichkeit, denn die Versorgungsanschlüsse sind zwar wichtig, aber für die Sachaltungslogik von eher untergeordneter Bedeutung. Lassen wir sie also separat.

Bauteilname und Bauteilwert

Beschriften Sie zunächst das Hauptsymbol mit den Textvariablen Bauteilname und Bauteilwert. Dazu verwenden Sie nacheinander die Toolbar-Knöpfe !N für den Bauteilnamen und !V für den Bauteilwert (value). Am Symbol platzieren Sie den Namen im Norden und den Wert im Süden. Es entsteht !BAUTEIL für den Bauteilnamen und !WERT für den Bauteilwert. Das Rufzeichen besagt, dass es sich um Textvarablen handelt. Der reale Inhalt von Name und Wert ergibt sich später.

Bauteilname und Bauteilwert

Bauteilname und Bauteilwert

Den Bauteilwert bringen wir unten am Bauteil an (Süden).

Behandlung der Versorgungsanschlüsse VCC und GND

Drehen und verschieben Sie jeden der beiden Anschlüsse wie im nachfolgenden Bild dargestellt und beschriften Sie sie mit der Textvariablen "Bauteilname" (gleiches Verfahren wie oben). Die Anschlussnamen können später mit [Entf] einfach gelöscht werden, wobei diese aber logisch erhalten bleiben.

none

Bauteile separat zusammenfassen

1. Schritt

Markieren (Fangen) Sie das Haupt-Symbol (das mit den sech Anschlüssen), indem Sie mit M1H im "Zeiger-Modus" ein Fenster über das Symbol aufziehen. Rechteck, Anschlüsse und Namen müssen komplett markiert werden! Am besten Sie ziehen das Fangfenster von rechts unten nach links oben auf. So markieren Sie alles zur Gänze, was berührt wird. Setzen Sie den Cursor an die Stelle, an der das Griffkreuz erscheinen soll (z.B. Mitte des Symbols). Drücken Sie jetzt die Tastaturtaste [y]. Der Dialog "Symbol zusammenfassen" erscheint.

noneBild: Der Dialog "Bauteil zusammenfassen"

Drücken Sie OK. Der Cursor verändert sein Bild und per Mausklick platzieren Sie das Griffkreuz. Das folgende Bild entsteht:

noneBild: Symbol mit Griffkreuz

Das Griffkreuz erscheint, die markierten Elemente werden so zu einem exportierbaren Symbol zusammengefasst.

2. Schritt

Markieren (Fangen) Sie das Versorgungs-Symbol (= die beiden Anschlüsse VCC und GND), indem Sie gleichermaßen mit M1H im "Zeiger-Modus" ein Fenster über das Symbol aufziehen. Anschlüsse und Namen müssen komplett markiert werden. Setzen Sie den Cursor an die Stelle, an der das Griffkreuz erscheinen soll (z.B. Mitte des Versorgungs-Symbols). Betätigen Sie erneut die Taste [y], um das zweite Griffkreuz zu setzen.

noneBild: Auch hier mit "Y" das Symbol zusammenfassen

Drücken Sie OK. Der Cursor verändert sein Bild und per Mausklick platzieren Sie das Griffkreuz. Das folgende Bild entsteht:

noneBild: Versorgungs-Symbol mit Griffkreuz

Versorgungssymbol als "Rest" definieren

Klicken Sie mit M11 auf das Griffkreuz und nehmen Sie folgende Änderungen in dem sich öffnenden Dialog vor:

none


Symbolnummer = 1, Einfügen= "Extra als Rest einfügen" (Versorgungsanschlüsse werden als "Rest eines Bauteils" im Schaltplan platziert) und Suffix = p für Power (Versorgungsanschluss).

Das Bauteil speichern

Markieren Sie nun das Bauteil und das Versorgungs-Symbol komplett, indem Sie ein Fangfenster über beiden aufziehen. Betätigen Sie die Taste [x] zum Exportieren des Bauteils in die Datenbank. Der Dialog "Bauteil exportieren" erscheint:

none

Wählen Sie einen Bauteiltyp unter einer bestimmten Bauteilgruppe und/oder erstellen Sie ggf. eine neue (1). Geben Sie den Bauteilnamen, hier LTC1392, ein (2) sowie den Hersteller (3). Geben Sie IC als Präfix ein (4). Das passende Gehäuse (5) steht ja von vornherein schon fest (ältere Versionen wählen es hier aus). Eine Bauteilbeschreibung (6) ist sinnvoll. Falls ein Bauteil kein Gehäuse bekommen soll, z. B. ein Referenz-Bauteil oder ein Schaltplan-Rahmen, dann lassen Sie das "Gehäuse:" - Feld leer. Nach Klick auf "Bauteil speichern" und Ignorieren eines History Eintrags, öffnet sich der folgende Dialog:

noneBild: Das neue Bauteil ist erstellt.

Nun befindet sich Ihr eben gezeichnetes Symbol inclusive Gehäusevorschlag in der Datenbank und Sie können es mit der Funktion "Bauteil Importieren" oder mit der Taste [Einfg] in Ihren Schaltplan holen. Es hängt an Ihrem Cursor und Sie können es beliebig oft absetzen. Durch drücken von M12 oder durch [ESC] hängen Sie es vom Cursor wieder ab. Wichtig: Die Versorgungsanschlüsse mussen über Menü: Bauteil/Reste von Bauteilen importieren... separat herein geholt werden. Daher hat das Symbol in der Browservorschau auch nur sechs Pins statt acht.

Zurück zu Bauteilerstellung

How to draw a reference symbol

Connections over several schematic pages and not visible signal islands of the same signal need to be connected by reference symbols. Please do the following steps to create a reference symbol:

1. Open a new project with an empty schematic page.
2. Draw the reference symbol with the help of the drawing tool .

3. Click with M11 on the pin name. (The "Change Texts" dialog appears).
4. Enter the pin name in the first field (text), for example SIGN-OUT. Press OK.
5. Double click the Pin, the "Change Pins" dialog opens. Untick the box "Show pin number" and tick the box "Is reference pin" like in the image below. Then press OK.

6. Highlight the whole reference symbol (drawing, connection) with the mouse.
7. Place the cursor to the spot where the handle shall appear (for example on the cross of the pin).
8. Press the [y] key.

9. Press the [x] key. The "Export symbol" dialog appears.
10. Enter "Reference Symbol to the "Select component type" line.
11. Enter a name for the reference symbol, enter properties if you like and press button "Save component".

Where can an exported (edited) component be found?

It plunges into the database and can be found by the name/parameters you had given to it or maybe by the package name. Maybe it is helpful to search only within USER components
(= the range of your components...)