Technology Library Editor

The Technology Library Editor dialog allows you to create an entry in the Technology library. It is displayed by clicking Home > Editors > Technology in eCADSTAR Library Editor.

Item   Description
Technology list   This section allows you to filter the technologies and add new technologies.
Filter   Allows you to filter the technologies.
  (Clear filters) Clicking this clears all filters.
  Name A drop-down list allowing you to filter the technologies, by name.
  Number of layers A drop-down list allowing you to filter the technologies, by number of layers.
Add technology   Displays the Add Technology dialog. This dialog allows you to add a technology to the technology library 
(Technology list)   A list of all current technologies.
Technology name   Displays the name of the technology. This value cannot be edited.
Number of conductor layers   Displays the number of conductor layers in the technology. This value cannot be edited.
Comment   A comment about the Technology.
  Allows you to toggle the display of board layers.
  Allows you to toggle the display of conductor layers.
  Allows you to toggle the display of dielectric layers.
  Allows you to toggle the display of non-conductor layers.
  Allows you to toggle the display of inhibit layers.
  Allows you to toggle the display of user-defined layers.
Layer Configuration tab   Allows you to configure the layers in the design. If the Conductor button is toggled off, non-conductor and inhibit layers are not displayed in the Layer Configuration tab.
  Layer name Displays the name of the layer.
  Layer type Displays the type of the associated layer.
  Soldering method Allows you to specify the soldering process.
  • Undefined: the soldering process is not defined. For thermal pads: if Undefined is selected, and Resist Check is selected in the Design Settings dialog, then the resist associated with the pad is not considered by the Online DRC process.
  • Wave: a bulk soldering process by which large boards can be soldered quickly and reliably during PCB assembly. This soldering process is typically used for through-hole components.
  • Single Reflow: the reflow soldering process is used only for one side of the board.
  • Reflow: a process in which solder paste is used to temporarily attach electrical components to their contact pads. The entire assembly is then subjected to controlled heat, which melts the solder and permanently connects the joint.
  Layer attribute Allows you to select from the following options for each conductor layer.
  • Positive: when a via that passes through the layer encounters an area fill pattern, the land is not set to a thermal or clearance land.
  • Powerplane: a conductor layer for which the whole area fill is set as one net. The Powerplane layer is used as a ground or power area fill in general use, and handled as a negative image layer in terms of manufacturing. Only thermal and clearance lands can be generated on the Powerplane layer.
  • Positive/Negative: when a via that passes through the layer encounters an area fill pattern, the land is automatically set to a thermal or clearance land which is defined in the padstack definition. This layer is used to make a multi-power design, and is also used to route track patterns of another net on the power/ground layer. When the packaging density is lower, or the number of layers is sufficient, the Powerplane design can be used. However, with the high board density and advanced high-level functionality, the Positive/Negative mix design is more effective for routing track patterns on the internal layer, and to create a multi-power design.
  • Track Keepout: a layer on which no surface mount conductor objects can be placed. This includes the following objects.
    • Pad/Padstacks
    • Route/Line
    • Area
    • Text
  Layer comment Allows you to add a comment for the layer.
  Associate Conductor Allows you to associate a selected user-defined layer with a conductor layer, using the Specify Conductor Layer to Associate dialog. Select the conductor layer and layer type in the dialog, and click Associate. Multiple conductor layers can be selected using the Ctrl or Shift keys.
Note
It is strongly recommended that a particular user-defined layer is not assigned twice to the same conductor layer using both Other and keepout layer types.
  Release Association For a selected user-defined layer or associated layer, the Release Association button allows you to release the association between the specified layer and all relevant conductor layers.
  • If you select a user-defined layer in the Layer Configuration tab, all associations with conductor layers are released, and the Layer Configuration tree is refreshed. Alternatively, right-click the user-defined layer and select Release All Associations on the assist menu.
  • If you select an associated layer in the Layer Configuration tab, the association is released between the layer that you select, and the conductor layer. Alternatively, right-click the user-defined layer and select Release Selected Association on the assist menu.
  Add Allows you to add layers to appropriate positions in the Technology Editor dialog.
  • If a conductor layer is selected in the Layer Configuration tab, the Add Layer dialog is displayed when you click Add. Insert a new conductor layer above or below the selected layer by clicking Insert Above or Insert Below in the Add Layer dialog.
  • If a dielectric layer is selected in the Layer Configuration tab, then this button is made unavailable.
  • If a User-defined layer is selected in the Layer Configuration tab, the System Layer dialog is displayed when you click Add. Specify the number of dielectric layers to add in the System Layer dialog and click OK.
  Configure System Adds a system layer to a selected conductor layer (outermost layer), using the System Layer dialog. See: Adding a System Layer to the Technology.
  Duplicate Duplicates a selected conductor layer (not an outermost layer).
  Delete Deletes a selected conductor layer (not an outermost layer) or user-defined layer.
Layer Mapping tab   Allows you to map footprint layers to the layers in the selected design data.
  Footprint layer box List of all footprint layers.
  Show footprint layers Show footprint layers that are able to map to layers in the selected design data.
  Layer mapping Map footprint layers and layers in the selected design data.
  Layer name The name of the layer.
  Side A For the mapped footprint layer, components in the design are placed on the top side of the board.
  Side B For the mapped footprint layer, components in the design are placed on the bottom side of the board.
  Layer comment Any comment for the layer.
Layer Display Order tab   Allows you to specify the order in which the layers are displayed.
  Conductor layer and associated layer Clicking this sets the display order to be by Conductor Layer and then by any layers associated with each Conductor Layer.
  Conductor layer Clicking this sets the display order to be by Conductor Layer.
  (Reset layer display order) Clicking this resets the display order of the layers to the default.
  Layer name The name of a layer.
  Layer type The layer type for the respective layer.
  Up Clicking this moves the selected layer up in the display order.
  Down Clicking this moves the selected layer down in the display order.

 

Related Topics
Adding or Deleting a Technology
Add Technology Dialog
Editing a Technology for the Board
Add Layer Dialog
System Layer Dialog