jmn's additions ===================== For alberta pc boards. Simplest way is to alter the T1 and T2 padstacks to have the correct drilling sizes as T1 and T2 is what is used in the DIP footprint library. The user.prt file in the layout executable directory is used to help layout decide what footprints to use. The tool file that alberta wants is equivalent to the (undocumented) .drs file. This file just gets created when you do the batch reports. Set output to gerber extended to avoid sending them an aperture file. If you want to merge two independently created layouts it is no fun since Layout seems to lack an import feature to do this.... Get the gcprevue program from apcircuits, use it to load in your .tap file, from which you get to make the drill rack. Read it in as a drill data file and use the auto_in.pdf format (I think - otherwise use the NCDRILL format). If you get this wrong the layer view will show it. Next, define your various top and bottom layer files and load them in, appylying whatever offsets you wanted to (Orcad data is 3.4 by default so you can use the auto format here). It will want to generate an aperture list. Let it. Now, in another window examine your .drs file and edit the drill rack manually to match it. Finally, define physical layers, save, and send to apcircuits. If you do this wrong I suppose the preview (F2) will show drill holes bigger than the encircling metal. This would probably get a bit more complicated if the layouts you are merging are made with different drill bit codes. I suppose this could happen if different programs made the original layouts. On auto-routing. Use the net spreadsheet to select the power nets and route those first. Then select everything else there and go to the route pass settings and reset the done flag. Autoroute again. It's a good idea to put your ref designators and maybe your values on the top layer in copper - as long as your board isn't too dense. There is some easy way to do this for all devices but I don't recall it now.. Perhaps from the library browser? BOOO's HELP FOR OrCad ===================== CAPTURE ------- Read the tutorial and do a few of the exercises. The tutorial is pretty good Don't forget to make connections to the outer world with headers, including Vcc, Vdd, in, out etc. And of course don't forget to connect your IC:s to power. Connect pins that are not in use to the NC-symbol WITHOUT a wire in between Don't use components from the DEVICE library since they have no names on their pins. When you create the netlist, use the layout option. If you check ECO, it will tell layout that the netlist is changed and layout will ask you if you want to use the updated netlist. LAYOUT ------ Go through the tutorial, but it is not too good. A common feature is that you have all options you can do with a component/wire on the right mouse button (RMB) NEW DESIGN - choose a technology file. 1bet_any.tch will do but have a lot of layers C:/Users/Borett/Borett.tch has fewer layers and works for APC - load netlist and save Now you have a ratnest of components and connections. We need to sort it out. PLACE COMPONENTS - Make sure Tool/Component is selected - press s (for select) - fill in component's name (eg R1 or R* if you want all of them) - you can now move the object(s) around and rotate them with r - Make a rough placement of your components ROUTING - mark window with View/DRC Box - autoroute with Auto/Route Window - check how much is routed with Window/Database Spreadsheets/Statistics - you can also manually route by clicking on net (select it) - you can rip up nets or connections with RMB (after selecting a net) - You can select a connection and then tell what layer it should be on by pressing that layer's number (eg 1 for top) - If you change layer while manually routing by pressing that layer's number the program will automatically place a via there. - you can also place vias with RMB COPPER POUR - select Tool/Obstacle - RMB/Insert - RMB/Modify - choose Copper Pour under Obstacle type Which layer you want to pour on The netname of the net you want the copper pour to be connected to. NB! Write the name with capitols - draw the area you want the copper pour to cover (eg if you want a ground plane over all of the board, make a rectangle around the whole board) - I changed the width of my power networks with RMB/change width and then did a copper pour over the whole board for my ground plane. DATABASE SPREADSHEETS - Here you can find and sometimes change all kinds of information. POST PROCESSING - Press the post process button - choose Setup batch From this table you can preview gerber plots from the different layers and you also tell which layers you want to have files from. For APC this is the top and bottom layer - select a layer (say top) and press the RMB - RMB/preview then Window/tile Now you can see what your layer will look like - Window/reset all to get back to normal view - In the setup batch table you tell which files will be generated by enabling them (yes in the enable coloumn) - Select a layer - RMB/Modify Choose Extended Gerber under format Check on enable if you want a file for that layer You can also choose the name of the file, rotation and scale etc - When you have modified all layers as you want them do RMB/Run batch The program will ask you if you want a drill tape and you do CHANGING DRILL HOLES APC only give you a few choices for the drill hole sizes that are free. If you want some other size you have to pay extra which is unnecessary. But your footprints probably have other sizes so you want to change the sizes. The free sizes are .0280 .0350 .0420 .0520 .0595 .0860 .1250 .1520 inches ---8<-----8<--- CUT FROM AN APC FILE ---8<-----8<--- Here is a guide to assist you in the selection of your drills. This is not intended to be taken as sage advice, simply put, it's come from first hand experience. Remember, while prototyping, give yourself a bit of extra hole size - it makes it much easier to remove the component (blue wire modifications)..etc. .028" - via and some TO-92 packages .035" - most IC packages .042" - IDC headers, IC's, 1N4000 series diodes, TO-220's, 1/2W resistors .052" - switches, stranded wire, molex headers .060" - swithches, large headers & inter-connects .086" - mounting holes in TO-220 packages, screw terminals .125" - mounting holes .152" - mounting holes ---8<-----8<-----8<-----8<-----8<-----8<-----8<-----8<--- - I noticed that our Molex headers need bigger holes than .028 :( - You change the drillhole sizes in the database spreadsheet Padstacks Find the drill hole you want to change and adjust the numbers to your convinience COPY YOUR LAYOUT ---------------- http://www.orcad.com/techserv/tn/tn69.htm SENDING YOUR ORDER TO APC ------------------------- You need to send If you used extended gerber for your files you don't need to send and aperture file.