File Menu
New
The New command creates and displays a new untitled design along with a dialog that lets you select initial design options. The dialog is shown below. By default, the new design has 4 layers and a working area of 12 inches by 12 inches. To change some of the design options later, you can bring up the same dialog with the Design Options… command from the Edit Menu.
You can make the working area any size equal to or larger than your PC board size. You can also define a Working Area Margin that provides an additional area surrounding your working area.
Open…
The Open… command opens an existing Osmond design file. Osmond design files should have a .osm extension.
Open Recent
The Open Recent command lets you select from a list of recently opened design files.
Import
Import → Setup…
The Import → Setup… command lets you read a setup file containing general information about the design such as number of layers, design rules, size of working area, etc. This is a text file that can be produced from an existing design using the Export → Setup… command. You can also edit it with an ordinary text editor.
You can also read an existing Osmond design file with this command. If you do, only the setup information contained in the design file is used. You can use this feature to clone the setup of an existing design.
Import → Library…
The Import → Library… command lets you read a Library file containing part type definitions. This is a text file that can be built either with the Osmond application or with an ordinary text editor. The format of the Library file is described in the File Formats section of this document.
Each library that you import is added to the library of the current design, thereby increasing the size of the file that must be saved. As an alternative, you can just Open a library in a separate window. The Library Parts window, which you view via the Window menu, gives you access to any part defined in any open design. This allows you to use any part in any library without the need to import the entire library into your design.
You can also read an existing Osmond design file with this command. If you do, only the part type definitions contained in the design file is used.
Import → Part List…
The Import → Part List… command lets you read a file containing a list of parts for your design. Each element of the list associates a unique part name with a part type which should eventually be defined in the Library file.
You can still import a part if the part type is not defined in any library. In this case, a placeholder part type is used and you should replace this with a real part type using the Replace Parts… or Replace Deferred Parts… command before you import the Net List.
The format of the Part List file is described in the File Formats section of this document.
You can change part types or add parts to a design by changing a part list and importing the new part list into an existing design. If you import a part list that is equivalent to the existing list of parts in a design, nothing will change.
You can also import an existing Osmond design file with this command. If you do, only the part list information contained in the design file is used.
Import → Net List…
The Import → Net List… command lets you read a file containing a list of signals for your design. Each signal contains a signal name and a list of pins that should be connected to the signal. The format of the Net List file is described in the File Formats section of this document.
If you import a net list into an existing design, Osmond will attempt to make the design consistent with the new net list. Note that this may require removing paths between pins if the design is changed.
You can also read an Osmond design file with this command. If you do, only the net list information contained in the design file is used.
Import → Part and Net List…
The Import → Part and Net List… command lets you read a file containing both a list of parts and a list of signals. This command is equivalent to doing an Import → Part List… followed by an Import → Net List… on the same file.
Import → Sub Design…
The Import → Sub Design… command lets you read a file containing a complete Osmond design, which then becomes a sub-design of the current design. The intent is to allow a larger fabrication panel to be built up by combining a number of smaller designs. The smaller designs can be identical or different. Each imported sub-design is given a unique sequence number, starting with 1. Once sub-designs are imported, the Select Sub Design… command in the Edit menu lets you select a sub-design by specifying its sequence number.
When this command is invoked, a dialog appears as shown below that lets you select a Multiple checkbox as well as X and Y offsets. If Multiple is not selected, the X and Y offsets are applied to a single sub-design. If Multiple is selected, the X and Y offsets specify the step-and-repeat spacing as multiple copies of a single sub-design fill the available working area. This is designed to ease the creation of a multi-design panel.
Import → Lua Script…
The Import → Lua Script… command lets you read and execute a script in the Lua language. Lua provides scripting and command line access to selected internal Osmond functions. See the Scripting and Command Line Interface section for a full description.Import → DXF File (inch)…
Import → DXF File (mm)…
These two commands let you read a DXF file into the current layer of your design. Because DXF files may have arbitrary units, two commands are provided: Import → DXF File (inch)… assumes that all dimensions are in inches while Import → DXF File (mm)… assumes all dimensions are in millimeters.
DXF support is limited. Only line, polyline, and text elements in the Entities segment of the DXF file are recognized. Each line and polyline element is drawn on the current layer with the current layer's default line width.
Import → PDF File…
The Import → PDF File… command lets you display the first page of any PDF document as a faint background image. This background image can serve as a design aid or as design verification. You can adjust the offset and visibility of the PDF image with the PDF Image… command from the Edit menu.
Import → Logo Image…
The Import → Logo Image… command lets you import an image that can then be placed on the design using the Text tool. The image is rendered using numerous straight paths so it can be translated to the Gerber commands needed for board fabrication. The image file imported should be a black and white PNG image.
Export
Export → Setup…
Export → Library…
Export → Part List…
Export → Net List…
These four commands let you export the current board setup, Library, Part List, and Net List, respectively, to output files. These files are text files and use the formats described in the File Formats section of this document. They can therefore be read with the corresponding Import commands described above.
Export → Solder Paste Design…
This command creates and allows you to save a new Osmond design file from the current design that gives you finer control over the creation of solder paste templates. Normally, when you export Gerber files, you also create solder paste template files that have entries that match the location, size, and shape of all surface mount pads in your design. There may be times, however, when this is inadequate.
The new design created by this command retains from the original design all the surface mount pads while omitting extraneous items such as traces and through hole pads. The new design can now be edited. You can, for example, modify the size and shape of pads or augment them with other pads as needed. Then, when you export Gerber files from this design, you will have solder paste templates that can be combined with the Gerber files exported from your original design to complete the package of files needed for fabrication.
Note: Make sure that you save the new design file in a separate directory. Otherwise, when you export Gerber files to make the solder paste templates, you will overwrite the Gerber files that you made from your original design.
Export → Gerber Files…
The Export → Gerber Files command writes all necessary Gerber files into a folder named Gerber Files in the same folder as your design file. A new Gerber Files folder is created if it does not already exist. The Gerber files conform to the RS-274X format.
When the command is invoked, a dialog appears as shown below. This dialog lets you select which layers will be exported and also lets you specify which (if any) of the layers will be mirror imaged. The manufacturing process usually requires mirroring of some layers. However, many board manufacturers can perform this mirroring themselves, so you may not need to bother with these options.
If you make signal planes using copper flood or signal plane layers, these are normally rendered using a combination of Gerber layers with different polarities, clear and dark. Because some board manufacturers are not able to handle this technique, a different rendering method is available that flattens copper floods and signal planes into a single layer. To select this method, check the Flatten Copper Flood and Signal Planes box. This method uses rectangles of various sizes to construct the copper flood areas, down to a resolution of 1 mil. Gerber files produced with this method will be substantially larger.
Note: Make sure there are definitions for all the alphabetic characters in your current library. Osmond uses these when creating the silkscreen Gerber files, which usually display part names.
The command also writes an Excellon drill file into the Gerber Files folder as well as a testing file that conforms to the IPC-356 format, and a file that provides pick-and-place data.
Export → DXF Files
The Export → DXF Files command writes several DXF files into a folder named DXF Files in the same folder as your design file. A new DXF Files folder is created if it does not already exist. The DXF files show part and pad outlines as well as the position of the holes. These files can be imported into a typical CAD program to produce fabrication and assembly drawings.
This command also writes a Hole Report file into the DXF Files folder that lists the number and sizes of all the holes used in the design.
Export → PostScript Files…
The Export → PostScript Files… command writes Encapsulated PostScript files of all board layers, including silkscreen and solder-mask layers, into a folder named PostScript Files in the same folder as your design file. A new PostScript Files folder is created if it does not already exist. These files can then be imported into other applications that accept Encapsulated PostScript.
With a printer of sufficient resolution, you may be able to produce transparancies that can be used directly to make your printed circuit boards. 300 dots per inch may be marginal but greater resolution should work well.
When the command is invoked, a dialog appears as shown below. This dialog lets you select which layers will be exported and also lets you specify which (if any) of the layers will be mirror imaged.
Note: Make sure there are definitions for all the alphabetic characters in your current library. Osmond uses these when creating the silkscreen PostScript files, which usually display part names.
Compare
Compare → Part List…
The Compare → Part List… command brings up a dialog that lets you select an external part list file for comparison with the internal part list. An alert will inform you if the internal part list is equivalent to the external part list. However, if the part lists are different, a text file will be generated showing where the two lists differ.
Compare → Net List…
The Compare → Net List… command brings up a dialog that lets you select an external net list file for comparison with the internal net list. An alert will inform you if the internal net list is equivalent to the external net list. However, if the net lists are different, a text file will be generated showing where the two lists differ. Note that net lists can be equivalent even if the signal names are different.
Close
The Closecommand closes the current design. If the design has changed since the last time it was saved, a dialog will appear asking if the design should be saved.
Save
The Save command saves the current design to the same file to which it was last saved. If the design has not yet been saved to a file, a finder dialog will let you specify where the new file should be saved.
Save As…
The Save As… command saves the current design to a new file that you specify in a finder dialog. This file becomes the current design file.
Revert
The Revert command reverts the current design to that of the last saved file.
Page Setup…
The Page Setup… command lets you change certain print options, the most useful being the orientation of the page and the scale.
Print…
The Print… command lets you print the current view of your design.
When you print, the current view is printed, including all visible layers. The current layer is always visible and other layers can be made visible or invisible through the Layers Visible dialog (invoked from the View menu). To print all the layers on different pages, go to each layer and print it in turn. Go to the Page Setup… command to change the scale. In general, what you see on the screen is what you get on the page.