Version 8

    This FAQ is no longer maintained, please use our dedicated Knowledge Base



    CircuitStudio FAQs

    Created by the element14 Software Technical Support Team. Contact us at



    1.    Is there an offline installer available for CircuitStudio?  No, we only support the online installer.


    2.    Can firewall block CircuitStudio from installing?  Yes, firewall can block the installation process.


    3.    What can I do if the firewall is blocking the installation?  CircuitStudio uploads using SOAP over HTTP (port 80). If the firewall or proxy is blocking it, it's most likely because SOAP is blocked as a protocol. Try Downloading the software from a different computer that is not blocked by firewall. You can also have your IT department open up the port to complete the download.


    4.    How do I create a local schlib for components I placed on the schematic from the vault?  The Vault components are intended for consumption only, not for modification, so there is no need to create a local library from them. Altium do proivde a vast selection of downloadable libraries you can install, use and edit from their design center.


    5. Is it possible to create a circular PCB in Circuit Studio?  It is possible to make circular PCB outlines, using SHIFT + SPACE to change corner mode while re-defining board shape.


    6.    Are delay Rules/ Line Matching Supported in CircuitStudio?  Length tuning can be done while routing. However there are no design rules for controlling the length - that is done by the user with the routed lengths displayed in the PCB Panel.


    7.    Can I use blind/buried vias in CircuitStudio?  Yes, you can. In order to use blind, buried or build-up type vias, the Drill pairs must be configured, with a drill pair for each layer-pair that a via spans. This can be done by using the Drill Pair manager which can be found under the Layer stack manager.  Go to home tab then click on layer stack manager. Once in Layer stack, click on Drill pairs. This will open the Drill manager where you can configure.


    8.    How do you convert special strings in Circuit Studio?  The option to convert special strings is found in the View Options tab of the View Configurations dialog. The View Configurations dialog is accessed from View>>Switch To 3D>>View Configurations, the L key on the keyboard or the Current Layer button to the left of the layer tabs in the PCB editor.


    9.    Does CircuitStudio support embedding STEP models into the PCB design?  Yes, you can embed the .STEP file model into a new footprint and place it into the PCB design.


    10.  What is the best way to do line matching in CircuitStudio?  Display the nets in the PCB panel and route them to the same length. The length calculation is displayed in real time.


    11.  How can I move an area of components and traces?  Go to preferences in PCB and set "Comp Drag" from "none" to "Selected Tracks", then use the Tools ribbon and Move -> Drag. If that doesn’t work you can also try the command Tools | Move » Move Selection.


    12.  Does CS support a database library .DbLib format used in Altium designer?  CircuitStudio uses integrated libraries. Dblibs can be converted to integrated library’s in Altium designer so they can be used in CircuitStudio.


    13.  How can I view different angles of the board using the 3D PCB mode? To move the board to any angle hold down the right shift key and a rotational icon will appear with the right mouse button rotate the PCB to the desired view.


    14.  How do you make a surface mount footprint? Is there an option for defining surface mount pads?  The SMD pad are created in the same way as through hole pads -  just on the layer desired either top or bottom but they do not have a hole size. Place pad – hit the tab key and edit the hole size to 0 and layer from multi layer to top layer.


    15.  Is it possible to make a 3-wire junction?  It is possible to create a 3-wire junction by clicking directly on an already placed wire(not the end of a segment) when placing the start or end of another wire segment. Here are some links to Altium Designer techdocs about auto and manual junctions.




    16.  Where can I edit the properties of multiple pins?  The properties of multiple pins can be edited in a schlib using the SCHLIB Inspector, View | Schematic | Inspector.


    17.  How can I move components without losing track to pad/via connection?  There is a preference (File » System Preferences » PCB Editor » General) in the "Other" region, set "Comp Drag" to "Connected Tracks." Then when editing, use the command, Tools | Arrange | Move » Drag.


    18.  Does CS have Keyboard shortcuts for features such as toggling via size or track width?  Min, Max, preferred via size is toggled with the 4 key or a favorite is set using SHIFT+V. Min, Max, preferred track width is toggled with the 3 key or a favorite is set using SHIFT+W. Press the Tilde key ~ while routing to see a list of available shortcut keys.


    19.  How can I mass edit a text size/style on the silkscreen or assembly layer?  Text on an assembly layer can quickly be selected using the PCB Filter(View | PCB | Filter), multiple selected items can be edited using the Object Inspector(View | PCB | Inspector).


    20.  I downloaded and connected a step model to the PCB file, how can I align it to the pads? The step model can be dragged and positioned in the X and Y axis in the 2D view of the PCB Library editor, the Z axis is set in the properties dialog as Standoff Height.


    21.  Where can I add snap points?  Snap points can be inputted manually in the 3D body properties dialog.


    22.  Is it possible to make the unrouted connections more visible or change their color?  It is possible to change the color of the rats nests unrouted connection lines for individual nets or a selection of nets using the Nets display of the PCB panel, View | PCB | PCB » Nets. Right-Click a net or a selection of nets in the PCB panel and choose 'Change Net Color'. Hovering over a unrouted connection line will make it more visible with live highlighting.


    23.  Is it possible to refresh the connections and eliminate the zig-zags after moving the components?  Use the command Tools | Netlist | Netlist » Clean All Nets to refresh the connections and eliminate the zig-zags. If that doesn’t work try: Select all the nets in the PCB panel then find the primitive PAD free1 in the primitive panel these are the items that need to be deleted. Highlight all the pads and then select them and then delete the object by clicking in the PCB window and pressing the delete key. Re run the design rule test and re sync the board with the schematic just in case you deleted any other objects in the PCB.


    24.  How can I enter text strings such as Title and Revision on the schematic title block? To create a special string, place a text string on the schematic or on the schematic template with a equals sign(=) before the parameter to to be displayed.

    Example special text strings for title and revision.




    25.  How can I switch layers during interactive routing without using a numpad?  SHIFT + Ctrl + Mouse Wheel to change layers while interactive routing...


    26.  How do you get the project to update the component footprint if the footprint in the library is changed?  Directly from the updated PCB library or from the project. If it is from the library just update the PCB using right click on the item. If from the project just push the updates after a compile to the PCB. This should change the footprint.


    27.  Is there a reference designator feature in CS to automate or re-annotate from PCB? In CS there is no tool to automate a ref des strategy. However, you can very much name the reference designators to whatever you like them to be on the PCB and push those changes back into the sch without the risk of losing the synchronization of the Sch and PCB. This is simply done by clicking on the update PCB action while you are in the PCB mode. This will take you through the standard ECO dialogue boxes to execute and document the changes. Once you’ve done that, everything will match up.


    28.  How can I add clearance rule to a plane? The rules apply to polygons (copper pour), but not to planes.  The best way to go about it is to convert the plane layer to a normal layer and pour polygon’s. You can apply rules to each polygon to get the desired clearance. It will be quicker and easier to control this way – Just allow for board edge pull back by setting up a keep out on the board edge.


    29.  Searched components in PCBdoc are highlighted and selected, how can I unselect the component?  You will need to clear your mask. You can do this from the view menu and click on clear at the far right or simply pressing SHIFT + C. There is a video about this on the e14 pages under the tutorial videos. That particular video is called "Cross Probing with Circuit Studio" Here is a link[iframe]=true&lightbox[width]=520&lightbox[height]=400


    30.  Is there a way to automatically set down a via and change layers while manually routing?  Use CTRL + SHIFT + Mouse wheel will change layers. Also the * key works but it's on the numerical keypad (not SHIFT+8). If you are not getting a via it's because there's something in the way or their via size is too big.


    31.  DXF file import is not working. The dialog says “Done”, but I don’t see any outline.  There are normally two main reasons why the DXF file doesn’t import correctly. The import may have completed, but at a VERY small scale. Try Zooming in to see if the image then shows up. If it does you may have to readjust your scale settings. 2- You may need to uninstall/reinstall the installation of TeighaX, the installer is located at C:\Program Files (x86)\Altium\CS\System\Installation\TeighaX_Setup_3.9.0.msi. TeighaX is a 3rd party utility used during import of dxf/dwg. Setting the correct scale and installing/repairing TeighaX should get things working.


    32.  It is possible to create a panelized board array in CircuitStudio?  It is possible to create a panelized board array in CircuitStudio but this is completely manual process involving copying and pasting the schematics and PCB layout multiple times then re-annotating. The board fabricator may be able to create the panel in their CAM tools.


    33.  Is there a way to print the schematics with the variant showing?  The schematics can be printed with the not fitted graphics by selecting the correct variant for the project or schematic prints in Projects | Generate Outputs or by making the compiled tab the active document and going to Outputs | Print.