Is there a way to update all sheet borders? When I make changes to the border file, the changes are not reflected on the sheets.
- I tried SETUP --> SETTINGS --> PROJECT --> BOARDS --> BOARDERS AND ZONES, but changing the border files and applying did not change the sheets.
- I have tried TOOLS --> UPDATE OTHER OBJECTS. I selected "Properties" and "Project" but the font size did not get updated.
- I have tried changing the border to a new/different border, restarting DxDesigner, then change the border back to the border I want to use. But it comes back to the old border.
For example, I changed the font size of a property in the border file. I go into DxDesigner try the above three things, but nothing changes. In the "Change Border" window, the border preview of the border is correct, but it is not updated when I inster it onto the sheet (see attachement).
Oh, those were probably added with the Cross Reference tool (formerly known as Scout), Adding Sheet Numbers to a Hierarchial or Flat Design is a TechNote that covers sheet numbering on designs. I've recently updated this TechNote to clean up the the references to Scout. Please let me know if you are successful or if the TN needs more work.
You have a couple of things to do here before you will get your design in sync. In the latest versions of DxDesigner for EE7.9.3/PADS9.4, EE7.9.4/5 and PADS 9.5 we introduced a new auto variable (the properties that begin with@) called @PRINTORDER. This defines the sheet number as it will be printed rather than just the sheet number in a block. This, in combination with @SHEETTOTAL will allow you to display 'Sheet n of m' in your border, where n = @PRINTORDER and m = @SHEETTOTAL, you should not use the @SHEET variable any more.
The first thing to do is add this new property to your sheet border symbol and delete the @SHEET property.
Save the symbol in your library.
Now update the symbol in the design, for a sheet border symbol there is only a very small bounding box defined, usually in the left hand corner of the sheet, due to this you will not see the 'out-of-date' indicator (if you have Flag out of date symbols switched on in your design) because the indication is given by highlighting the bounding box. To see this indicator zoom out further than the sheet extent, you should see a small red rectangle. Select the sheet border make sure it is enabled in the selection filter) and do the update. Check you now have @PRINTORDER on the symbol.
Once you have updated the sheet border across the design run Tools - Update other objects - and check the Properties and Print Order options.
This should bring the sheet numbers into line.
You can also display the print order value in the navigator by setting the following in Setup - Settings - Navigator - Label Format = $(Name) ($(Number))
This will display in the navigator like the picture attached.
Also see this thread
And watch the tutorial on SupportNet
and this video
Navigator.PNG 9.1 KB
Ok, so I found a way to get the borders to update. If I open the border in the Symbol Editor rather than in DxDesigner (just opened the text file). After I make a change, DxDesigner allows me to "Update Symbol."
Is there a way to update symbols that are modified outside the Symbol Editor? I changed the text size in all my symbols using a text editor, opened my schematic, and "Update Symbol" is empty.
Anyway, the page numbers are correct and "Update Other Objects" populates @PRINTORDER and @SHEETOTAL correctly. Now, I'm onto another problem. I cannot get nets to connect to my hierarchy blocks. here is what I did:
- I created a block
- Edited block and added pints
- Selected blcok and clicked Edit --> Push
- Drew / Pasted Schematic complete with net names and off-sheet arrows
- Tried to connect nets to block on the toplayer
- Received "Note 1066: Cannot short net"
I'm sorry about asking basic questions. Dx is not my normal envirnoment. Short schedules don't usually allow for software learning curves! I appreciate the help,
EDIT: I found an article here, that described adding ports to Setup->Settings-->Projects-->Board-->Special Components. As I mentioned, this is an existing schematic and I do not find any of the other nets in the Special Components (only GND and PWR).
On your first question, the update symbols works on the timestamp in the symbol definition file, the line beginning with |R so unless this is changed DxDesigner is not aware of the symbol updates.
On your second issue, generally you should do the following when creating a block symbol:
Set up your port symbols in Setup - Settings - Boards - Special Components. We provide some appropriate symbols in the Basic library.
Once you've done this you can create a block at the top level, add some nets and name them, this adds pins to the block with the same name. Then do push block and the nets and hierarchical connectors will be added automatically.
If you're working the other way, bottom up then you can do this in two ways, create the lower level schematic, add the ports and use Tools - Generate symbol to crate the block symbol. Or, as you have done create a block and add pins manually in the editor, in this case ensure the block symbol you create has its bounding box up to the pin extents otherwise you won't be able to connect to the block symbol.
Thank you for the response. I am working to implement your suggestion, but why are none of the other block's nets listed under the Special Components? There is about 10 other blocks that were done previously in the old revision.
The special components just list the symbols you will use for creating connectivity, in the case of hierarchical design you need to define the symbols you will use to connect the top level nets with the lower level nets through the block pin. In the case of hierarchical blocks you must define a port symbol (which is a 'Pin Type' symbol in DxDesigner terms). You should define a symbol for input, output and bidirectional port types (con_hier_i, con_hier_o and con_hier_bi are the supplied ones but you may create your own).
These pins estblish the connection through the hierarchy but other than that they do not have any other reference to the nets in other blocks.
I really appreciate the help, no I see why it wont connect. In Special Comonents, I have most of the ports set to builtin* (note, this was done by the previous designer). This is confusing because all the off sheet connectors in the schematics are arrow_*. When I push, I get erros that built* is not found. When I try to change the Special Components, no ports are found in the dropdowns.... including builtin*. The arrow_*.1 files stored in the directory with all the other components (*/<project>/Symbol/sym/), I've also tryed placing the arrow_*.1 files in with the blocks (*/<project>//sym/). The arrow_* symbol is set to ANNOTATE.
Why are the ports symbols not showing up when I browse in Special Components? And why are builtin* not showing up aw well (they are stored in C:\MentorGraphics\9.5PADS\SDD_HOME\Libraries\discretes\sym)?
You must define the specific symbol for each port type and they must be pin type symbols not annotate, annotate are used for inter-sheet connections though they are not strictly necessary. Your special components should look like:
You cannot use wildcards.
Ok, sorry I was trying to get out of typying all the filename:
The builtin* are the same... builtin:in, builtin:out, builtin:bi etc. and they all corrispond to the correct port.
The port symbols must be pin types to show up in the list. The error message is telling you they don't exist or the library pointer is incorrect.
Robert, I appreciate your responses and patience.
I think I am getting there. I have the ports generated when I click Push (had to add the common library to the Symbol Libraries in the Settings). I have connected the ports to the approperate nets/buses. On the schematic that has the block symbol, I am still unable to connect nets/buses to the block symbol (see attachement). I tried naming the net on the schematic the same as the net in the block (and block's schematic).
block_nconnect.png 103.2 KB
I suspect this is an issue with the bounding box on the symbol as indicated in an earlier post. Make sure this extends to the edge of the pins. Check the symbol editor manual for more information and also check the pins are on the correct grid.
If you think training is expensive, you should try ignorance!