Is there a way to place smaller bus entries? I find that the normal size interferes with placing other stuff nearby:
Manually adding a 45 degree wire where I want the bus entry to be, does not work as it does not connect to the bus:
@DavidR I had the same hiccup when working on one of my schematics.
What I did to get around it was to draw a line then drag it into a diagonal.
For clarification, the one diagonal line in my case was the master clock and not part of any bus.
I could have turned A13 and A14 the other way, but this way looks better.
In 5.99 and 6.0, diagonal lines are not the same thing as bus entries! If you just draw diagonal lines, some things like ERC will not work correctly.
There is no way to change the entry size right now; please file a feature request for it
What is the process for filing a feature request? The gitlab issue template seems to be geared towards defects.
I would change the grid to 25 supposing the current grid is 50. It is recommended to stick to the 50 grid but why not to use the 25 if it is there and it is useful for this case?
It doesn’t matter, just leave off the Steps to Reproduce part and describe the feature request. The exact version info is needed anyway. Someone will mark the issue as a feature request/wishlist item.
1 Like
eeschema in v5.99 already supports smaller bus entries but there just isn’t a way to create the object yet from within the GUI (that would be the feature request).
There is a workaround right now which relies on the ability to paste s-expression text elements as schematic objects.
The below will generate a bus entry with a size of 1.27mm x 1.27mm (i.e. 50mil x 50mil). Just copy the below text and in eeschema (v5.99), do a “Paste” and you’ll be able to choose where to paste it.
(bus_entry (size 1.27 1.27) )
Video better than 1000 words:
bus_entry_creation
Final result:
5 Likes
Heh, I can see everyone has their own ugly solution for this 
Actually I think this is a bug - why would bus entry connect to anything else than a bus?
Because a bus connects a bunch of pins on one side to another bunch of pins on the other side. The bus entry must be connected to a pin. The wire allows to extend that connection, making at the same time a more readable schematic.
It also allows the connection of the bus to more than one symbol on one side, for example a bus from a microcontroller/fpga to two memory chips.
Yes, sure, but what about the other end of it? I understand it’s messy from programming side of things as you can rotate bus entries, but one side of it should be connected, just to a bus, no?
Wire connecting to a junction of bus and bus entry makes no sense in my opinion i.e. I have this pic in mind:
That scenario should throw ERC warnings. You need a bus entry on MUX.SCL to keep them separate.
Hi David,
A better workaround would be to reduce the grid size to place the wires closer together.
-
Select the “wire to bus entry” option
-
Right-click and select the grid size as 10 mils
-
As you can see the wires can now be placed closer to each other.
-
If connections are an issue then select the “Place junction” option and use junctions to ensure a connection
-
Generate the netlist to see if all the required connections are done.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.