Check project
From IBF-Wiki
Also see Realtime design rule check
The check-routine will be started automatically after clicking the 
button beneath the icon 
You can also click in menu "File" on menu item "Check Project".
The dialog "check project"
Check components without a package, packages without components, short circuits, open circuits etc... Sometimes these situations are wanted or necessary. For example, if you only want to draw a PCB without having to think about drawing a schematic first.
Nevertheless, to have everything proceeding the right way, you can use this function.
The result of the check
After pressing the "Check" button, all Design-Rule-Check-errors and Electrical-Rule-Check-errors will be displayed in an error list.
You can also save this list as a text file called TARGET.ERR into the current working directory. Doubleclick upon a certain line in the error list to fade out the list and get the error highlighted in the canvas by error markers.
Clicking M11 on an error marker will pop up a window with a short description of the design error. Display the initial list again by clicking the button top left of the canvas "Show error list again". The display of the design errors can be disabled by deactivating layer # 28. The Reorganisation command makes all error markers disappear.
After all errors are corrected, TARGET 3001! shows (for example) the following list:
0 Bridges
5 Vias
211 Drill holes
Minimum drill hole diameter: 0,6 mm
Minimum distance between drill holes: 0,3 mm
Minimum annular ring of solder pads: 0,235 mm
Thinnest track width: 0,3 mm
Minimum signal distance: 0,25 mm
PCB size: 160 x 100 mm
The meaning of the error messages
The following error messages might occur during the execution of the Electrical-Rule-Check:
Missing package
The schematic drawing contains a component which requires a package. The package however is missing on the PCB. Please place the missing package on the PCB.
Unfinished signal
The schematic requires connections which are incomplete on the PCB. Either individual solder pads of the signal are not connected or the signal is made of two or more signal islands. For checking, activate the pointer-option Mark signal islands 
When you click now M1 on a track, you can see exactly where the signal flow stops.
The first image shows a track which isn't connected correctly in the middle of pad 1. Optically this track is touching the copper thus seeming to be connected. In fact two separate signal islands are created which aren't logically connected to each other. Please see the correct connection in the following image:
Tracks are "sensitive" only at their endings. Whether TARGET 3001! recognizes two tracks as "connected" depends on the setting of the grid. See the following image of the X-ray view of a track:
TARGET 3001! recognizes the track to the right side as "not connected" (see arrow), though their segments touch. The centers of their endings mustn't be placed more than half a grid apart from each other. Having lots of alerts in this respect we recommend to set the grid not too narrow.
Besides: Groundplanes in the layout do not carry on a certain signal. A groundplane is only supporting an existing track. See Groundplane.
.
Power without supply
The power supply connections of components are connected to a signal, but there is no power connected to the PCB. Usually, some pins of a connector are assigned to Function=Supply.
Lets say you have a 7805 and a 7400. The 7805 brings the power to the 5V net, whereas the 7400 is a consumer for power. So the 7805 has a pin set to function "supply" and the 7400 has two pins as power consumer called "power" (5V and GND). So "Power without supply" means a net has a power consumer connected but no supply. If the power comes to the net via a connector, set the respective pin of the connector to "supply".
Power signals are normally not handled with buses.
.
Output error
An error message referring to the schematic. One signal either is fixed to several output pins or to an output pin and a supply pin. In other words: several output pins are connected to a signal at the same time or to an output pin as well to a supply pin.
.
Island without Ref Pin
Error message of the schematic. The signal in the schematic consists of several signal islands which optically seem to be connected. The connection in fact must be effected by reference symbols or by buses. If the error message appears nevertheless, please set the highlighting mode by the use of to "mark the signal island hit" and highlight by M1 all islands of a signal after each other. Danger: this error message might point at a short circuit in the schematic. Example: at a resistor both pins are connected to the same signal. TARGET 3001! recognizes two islands of the same signal and the autorouter would short circuit the resistor with other signal tracks. For localizing this error please highlight the complete signal by the use of the binoculars ("Find and select a Component or Signal"). Check the schematic in any case when this error message appears after using the "Check project" function. If you really don't find a different signal island, then please search for "orphan" signal track pieces, which might lay under an already existing signal track. Use keyboard key [s] (for select) several times when the cursor is close to a suspicious spot. Different elements being close to the cursor will flash though eventually invisible because covered by another element. If it flashes, press Enter and then delete it.
Only inputs
There is no defined voltage level on a signal, because only inputs are connected (signal is flowing).
Open input
An input is flowing. Input pins of unused symbols must be connected. In case that the pin should really be unconnected, set its function to NC (not connected).
Short circuit
A pin on the PCB is connected to a different pin as required in the schematic. This is not a Design-Rule-Check, short circuits caused by crossing tracks and distance violations, are not recognized here.
Pin without a solder pad
There is a solder pad missing on the PCB for an existing pin in the schematic. Maybe you have deleted a solder pad afterwards from an existing package or you have used the wrong package.
Multiple supply
A signal is connected to several different power supplies.
Not connected
In the schematic a pin is not connected. Maybe it shall not be connected! To avoid this error message (better: Warning message) please set the function of the schematic Pin to NC (=not connected) in the Change Pins dialog:
More signal islands than reference symbols
Every signal island must show its ownership visually to a signal through reference symbols or through a connection to a bus. In this case, at least one signal island is not connected to a reference symbol. Click on each of the signal islands with M1. Hereby, the tool Mark signal island completely must be selected. This error could also be named as double signal name!
Component outdated
There is a more recent version of a symbol or package in the libraries than the one used in this current project. Using menu option "Search and replace component shape" in menu Components allows an update of components within your project. For the symbols the property "LAST MODIFIED" is compared, for the package the property "LAST_MODIFIED_PACKAGE" is compared.
Symbol/Package unknown
The symbol or the package can not be found within the libraries. For the check of the symbol TARGET uses the catchword under which the component was found when trying to import it and the property "COMPONENT_LIB". For the package the properties "USED_PACKAGE" and "USED_PACKAGE_LIB" are checked.
Spacing violation
A spacing violation occurs, if the copper of a different signal comes too close to the copper of the element in question or if it touches it. A spacing violation can be a short circuit in other words a short circuit in any case is a spacing violation. That means that the auras of different signal can overlap without alert which is correct. The minimum spacing of a copper element of a signal to all other copper elements of a "hostile" signal must be bigger than the biggest value out of the three:
- the minimum spacing in the "Check project" dialog
- the minimum spacing of the signal itself
- the aura of the element
If your layout according to the rules of a PCB manufacturer gets checked against e. g. 0,15mm general signal spacing, the security needs of signal "240V" indeed might be higher. Close to signal "240V" a wider minimum spacing needs to be defined in the signal dialog . If a track "+5V" (mainly located in a low volt area of your layout) also touches an area of line voltage then the "+5V"-tracks in this area should get a bigger aura.
The following images show 2 "hostile" elements and their auras:
Image 1: A soldering pad to the left and a track segment to the right
Image 2: Track segment touched by M1H for showing it's phantom lines...
If spacing d between the elements is smaller than the parameter in the "Check project" dialog, TARGET 3001! alerts a spacing violation. The track to the right might be OK with the distance to the pad. The pad on the other hand has a bigger aura which overlaps the track. From the Pad's point of view the spacing to the track is too small.
Note: Use these error messages to check whether your circuit has short circuits. If both pins of a resistor are connected to the same signal, a signal island is created. The autorouter therefore short-circuits the two solder pads of the according package symbol.
Component outline defective
This message appears, if the outline of a package or a symbol drawing is not closed properly. Make use of the hash-key [#] for X-raying your drawing. All frictions get visible quickly:
Image: Component outline defective
Design-Rule-Check error messages
Most of them are spacing violations or tracks that are too thin. TARGET 3001! regards the values entered in the DRC dialog as well as the properties of signals "MinimalWidth" and "MinimumSpacing".
Package Overlap
Two packages are overlapping. If a package shall be excluded from this check (e.g. if the PCB outline itself was imported as a "package", it would have conflicts with all other packages), then this component must get the property "IGNORE_OVERLAP" with the value "YES".
Width of the rest ring of a soldering pad
If the soldering pad diameter is 1 mm and the drillhole diameter is 0.6 mm, a rest ring of 0,2 mm results. As long as a rest ring remains at all, a plating through happens. A drillhole without rest ring thus doesn't get galvanised (=no plating through).
Spacing between drillholes
If the distance between two drillholes (center to center) is e.g. 1 mm and the drillhole diameters are 0.8 mm and 0.6 mm, a spacing of 0.3 mm results.
Wrong signal at clamp: CMP / Pin X "Sig$1"
Error message concerning cable harnesses. The component in question has property "IS_CLAMP" activated. To a certain clamp signals are connected, which are recognized an not belonging together e.g. "1.1", "1.2", ... "1.99" etc.. In case you do not intend to check clamps or cable harnesses, delete the components property "IS_CLAMP" or switch off the checking of the "Clamp assignment" in the Check project dialog.
Track segment not straight
This is a warning only, no error. It just tells that a track segment is not in the 45° angle grid. E.g. it has an odd angle of 17.26°. So it works, but might be a matter of esthetics.
File "C:\Programs\ibf\CounterParts.txt" missing
Error message concerning cable harnesses. Set in Settings (Registry) the entry "Cable functions in main menue" to "No" (position 8 from the bottom of the list)
Check - Aura - Track Spacing
The Aura is the security spacing a signal has towards a groundplane you might consider to create. The Standard track spacing (PCB) is the spacing a signal in general at least shall have towards another signal. Aura and Standard track spacing can vary e. g. if you would like to have a slightly bigger aura around pads for making soldering easier than you need to have alongside the tracks. TARGET 3001! offers setting options in the "Object inspector" which you open by menu "Settings/Settings (Project)..." The following settings are predefined as default:
TARGET 3001! uses these settings as "normal" signal properties in the schematic.
These values are overtaken to the layout at first but they can be adapted at any time.
When placing tracks you'll see a phantom image having hatched lines aside. This hatched lines represent the higher one of both values, by default the "Aura". If you set the value "Standard track-spacing (PCB)" higher than the value "Aura width", then the hatched line represents the standard track spacing.
In menu "Action/Check project..." to the right you see the field "Standard track-spacing" preset by 7.87 mil. The aura shall not be regarded in this checking situation, the box remains unticked:
In the check result TARGET 3001! marks all spots, where two varying signal leading elements have spacing to each other smaller or equal 7.87 mil. Whether the aura of one of those touches a signal element (e.g. a track) is disregarded according to this setting.
The following image might illustrate the situation. Starting from the center of the image you see two signal tracks, the upper one highlighted so that the manually set aura of 11.81 mil can be seen in hatched line. It touches the track beneath (red). Predefined is a minimum spacing of 7.87 mil against which the project now gets checked.
Situation 1 leaves the aura disregarded which does not lead to any error message, because the minimum spacing (7.87 mil) between the signal leading elements is kept. Shall the aura be regarded, the box in the check project dialog needs to be ticked see situation 2. Now TARGET 3001! alerts a spacing error because the aura of the upper track touches the copper of the lower track.
.