| Author |
 Topic  |
|
|
Boris
United Kingdom
34 Posts |
 Posted - 28 Jan 2009 : 17:28:25
|
Please could you tell me how you create a star point in a schematic layout. I have 20 different nets that I need to join at one star point then have one net leaving the star point to a component pin. Do you need to make up a special component which will be recognised when translating to the PCB?
Boris |
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 28 Jan 2009 : 18:30:49
|
Type "star" into easy-pc help file.....
|
 |
|
|
Boris
United Kingdom
34 Posts |
Posted - 29 Jan 2009 : 09:44:52
|
I have tried that and all it talks about is the PCB side. There is no mention of what you do in the schematic to create a star point.
So if I have nets A,B,and C in a circuit diagram that I wish to join to a star point and come away from there with net D, how do I do it?
Boris |
|
|
|
Peter Johnson
United Kingdom
498 Posts |
Posted - 29 Jan 2009 : 10:41:08
|
At present the assumption is that the nets will be separate in the schematic, and labelled as to their function, e.g. AnGnd and DigGnd.
There's no special provision in the schematic for a star point, so if you do need to represent the nets joining in the schematic, then you will need to create a schematic only component for this. You will need the same number of connection points as the total number of nets, including the one leaving the star point.
In the pcb the nets will have to be joined manually, as at present it's only free pads that can be designated as star points. That means that specific star point components aren't possible.
As far as I'm aware, yours is the first request for an item like this, so I don't know how any other users with a similar requirement have solved it. |
|
|
|
Boris
United Kingdom
34 Posts |
Posted - 02 Feb 2009 : 16:38:18
|
I think I have found a way of doing this.
I created a symbol with 4 connections (3 in 1 out).
I created a pcb symbol with four pads close together but not violating. I made the silkscreen shape of the pcb component diamond shape to represent a star....how sweet!
On another layer (a non-electrical general layer) I put a small block/shape using the 'Add Closed shape' command and filled it solid and placed it on top of the star point. The symbols can now be mapped as usual.
The circuit diagram can be created with all its separate nets as normal.
Translate to PCB and route away.
A DRC check will reveal no errors since all nets are separate and all clearances are correct and the block on the general layer is ignored.
When you send the Gerbers off to the PCB manufacturer tell him to plot the track layer and the general layer together to create a composite copper pattern which will show all the relevant nets joined at the star point.
The danger here is fogetting to plot the two layers together!!!!
Another way: -
In the PCB symbol for the Star Point the pads can be joined together by lines or a block placed on an electrical layer(s) of your choice.
The layout can be routed as normal and can be plotted out as a single Gerber as usual. However: -
A DRC will now show up track/pad to shape violations for the component on that layer(s) and if you have a lot of star points, for some reason, there will be a lot of errors to wade through before choosing to ignore them and go ahead and plot the Gerbers.
I know it is not the best of solutions but at least it does work.
Best regards,
Boris |
|
|
|
tcrouse
33 Posts |
Posted - 18 Mar 2009 : 17:59:31
|
Another solution is to use a bus, and use a common net name for all the connections. Then you can move the traces around in the PCB as you need to without getting any violations, plus no special instructions to the board house.
Best Regards
Tim C. |
|
|
|
Boris
United Kingdom
34 Posts |
Posted - 08 Apr 2009 : 15:45:07
|
Hi Tim,
I don't see that at all because as soon as you use a common net name then all the connections are joined together which is what I don't want. I need to route individual tracks form various places back to one point. If they have the same name then I won't know if I am linking up all the analogue grounds together or a mixture of analogue and digital and a host of other things.
Many thanks,
Boris |
|
|
|
Dave Lovell
United Kingdom
3 Posts |
Posted - 08 Apr 2009 : 19:05:46
|
| I did this several version of Easy-PC ago, so there may be better ways now. I did as you did with a Star component which can be DRC with poured copper planes. Then save this version for possible future revision. Finally, simply connect the pins of the Star component in the PCB editor with an "add track", all the nets become one, and a final DRC is still possible |
|
|
|
remi
United Kingdom
101 Posts |
Posted - 09 Apr 2009 : 10:28:05
|
| just out of curiosity is designing a circuit with a star point outdated or does it gives any good noise result? |
Edited by - remi on 09 Apr 2009 11:16:10 |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 09 Apr 2009 : 14:16:31
|
Quite honestly, from a professional point of view, with the costs of 4 layer PCB's these days, any "critical" cricuit would always be done on 4 layer. This completely negates the need for star points so long as the inner layers do not become too perforated. Also in these days of EMC, 4 layer is really a pre-requisite.
All this really makes star-points old-hat  |
|
|
|
Peter Johnson
United Kingdom
498 Posts |
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 17 Apr 2009 : 20:17:51
|
Well spotted Peter.... Star point your power planes .... the things we do naturally without even thinking about it.
Ok so there are is still a case for it...
|
|
|
|
shadders
United Kingdom
224 Posts |
Posted - 16 Aug 2009 : 13:11:58
|
Hi,
Just read through this forum text - which is opportune as i have this requirement too.
A question i have (not got to this part in my design yet) : Can you in the PCB editor connect the Digital Grounds and Analogue Ground using a star connection ?.
I would prefer not to go through the creation of a symbol in the Schematic designer.
Second question : Will the version 14 provide for a star connection in the schematic ?.
Thanks.
Regards,
Richard. |
|
|
|
Peter Johnson
United Kingdom
498 Posts |
Posted - 03 Sep 2009 : 17:49:49
|
Sorry shadders, been a bit slow picking this one up. If you look up star point in the help section, there are detailed instructions on how to create and use them in a pcb design.
It's a bit tricky drawing a schematic to show exactly where a star point should lie, as you can't use any labelled connections, but one way would be to use different net names, then where you wanted to join them, don't add a connection, as that will just merge the nets. Instead add a line (which will look like a connection, but isn't), but show the net names on the connections either side, and use free text or a text callout to label the star point.
At present there's no way to designate a star point in the schematic which will link to the pcb. If you'd like it added to the wish list, drop a request into the support desk, including your customer reference number. |
|
|
|
shadders
United Kingdom
224 Posts |
Posted - 09 Sep 2009 : 23:57:28
|
Hi Peter,
Thanks for the reply. I checked out the star point in PCB - it seems easy enough to accomplish. Thanks.
I will see how this proceeds - so probably will not request this as a new feature. Thanks again for the reply and assisatnce.
Regards,
Richard. |
|
|
|
davethesteam
United Kingdom
10 Posts |
Posted - 09 Feb 2010 : 19:48:02
|
Hi all,
I need to create a schematic with a star point and be sure that the DRC will find the missing connection if the PCB star point is not matching. I have 'bodged' this on all my previous PCBs and would really like to be sure I don't miss the joining of the star point. I've not missed yet but statistically the latest revision of my most expensive board is going to be the one
I really would be happy to see this work properly, I'll put a request in.
David
|
|
|
|
Peter Johnson
United Kingdom
498 Posts |
Posted - 10 Feb 2010 : 14:36:31
|
| Well, this has been logged as a request for V14, but as with all new features, there's competition for development time, so that's not an absolute guarantee. However, this thread does demonstrate a need, so that's bound to help! |
|
|
|
636steve
United Kingdom
14 Posts |
Posted - 21 Mar 2014 : 11:25:14
|
| Was this ever added to a later version as I have a need to do this but cannot get anything to work without creating a drc error in the pcb. |
|
|
|
Iain Wilkie
United Kingdom
1015 Posts |
Posted - 21 Mar 2014 : 13:29:08
|
Yes, you can have star points in schematics now as well as the pcb .... Certainly in V17
Iain |
|
|
|
636steve
United Kingdom
14 Posts |
Posted - 21 Mar 2014 : 13:59:01
|
Worked it out now
cheers |
|
|
| |
Topic |
|
Star points in schematic