| T O P I C R E V I E W |
| tswelectronics |
Posted - 12 Nov 2009 : 17:51:44
Hi all.
I really like the layout pattern tool but it seems sometimes to get things a litttle bit wrong. It can save a lot of work but I find myself worrying about using it with any complex patterns because I just cant be sure it did it.
Is there any tips on what makes it work best or any little gotches that will help get the most out of this really useful tool.
Thanks
Trev |
| 19 L A T E S T R E P L I E S (Newest First) |
| Iain Wilkie |
Posted - 31 May 2012 : 20:18:52
Well ... Was it fixed ?? I have just tried this again although the components are copied and applied, there are no tracks or vias copied just all the nets .... no match errors generated ...
If instead of selecting the "group" to be copied to the clipboard, you select the group by framing and select all ... so that everything is highlighted, then tracks on top and bottom are created when layout pattern is applied, however ALL internal layer tracks are missing !!! .... so frustrating
Ok ... making discoveries here ... what will NOT copy are the following ...
1 Any track that is effectively "dangling" ... i.e it one end ends on nothing.
2 Any via that drops onto a copper pour plane e.g. a via to a ground plane.
If this could be fixed we could be some way to a better result from this tool.
Iain
|
| Peter Johnson |
Posted - 04 Mar 2010 : 13:31:58
With a lot of help from Dave (dgeorge), we've confirmed a bug in the apply layout tool. Barring unforseen events, it should be fixed in 13.0.7, though when it's ready, anyone who's got a problem is welcome to ask for an early fix. |
| Iain Wilkie |
Posted - 03 Mar 2010 : 09:14:03
This is the "old" way of doing it .... i.e. before the apply pattern tool. It can sometimes fail also if the net numbering gets out of sync between sch and pcb. But you have been lucky. The last one I did using this method had 8 complex sections.... 6 of them replicated ok, but the last two were all mixed up and needed careful editing.
I have used the apply pattern tool a few times and have to admit it is not perfect and some nets/vias seem to get left out. However copying to clipboard seems to help.
Iain |
| dgeorge |
Posted - 02 Mar 2010 : 21:37:08
I have found a work around.
1. Eliminate all but one channel on the schematic and the PCB.
2. Lay out the PCB for one channel.
3. Copy and paste the PCB channel multiple times on the PCB.
4. Copy and past the schemati channel multiple times on the schematic.
5. Modify both the PCB to add common power and ground tracks. Modify both the schematic and the PCB to route separate input and output signals.
This procedure worked for me like I would have expected the Layout Pattern Tool to have worked.
I did not expect that this would maintain correspondence between the schematic and the PCB because the schematic design changes were never fowarded to the PCB. But for some reason, perhaps a simple sequential ordering one, this maintains a correct correspondence between components on the schematic and components on the PCB even for the channels that were added separately on the schematic and the PCB.
I have forwarded the project to you for your assessment if you care. However, it is now complete and any difficulties I was having are long overwritten. You could eliminate two of the three channels on the PCB, then forward design changes from the schematic to re-layout those two channels, then attempt to apply the layout pattern of the first channel to the other two and see if it works flawlessly for you. |
| DavidM |
Posted - 02 Mar 2010 : 17:04:30
If this really is proving as frustrating as you describe, and you have a repeatable case (which sounds likely from what you say) then we would of course be happy to investigate further if you are able to send the relevant design files to us.
There is usually a reason for things not working right, and its always possible that the reason in this case is that we need some correction in the code, although its rather hard to determine this for sure in the absence of solid data to reproduce the issue.
David. |
| dgeorge |
Posted - 02 Mar 2010 : 07:06:33
Here's a challenge.
1. Make a schematic of "one channel" in a multiple channel system.
2. All channels use common Vcc, Vdd, and Ground.
3. Assume each channel has its own inputs and outputs separate from the other channels.
4. Make a PCB layout of the first channel.
5. Select the components of that first channel and copy the schematic (Ctrl-C, Ctrl-V) of that channel to the schematic, thus producing multiple channels. Choose to connect Vcc, Vdd, and Gnd but choose not to connect the inputs or outputs.
6. Make groups of each of the channels on the schematic. De-select the option to make it a "schematic-only" group.
7. Forward design changes from the schematic.
8. Select the group from the first channel on the PCB. (You can also select the entire group including tracks and vias on the previously laid-out PCB for channel 1.
9. Use "Apply Layout Pattern" (ALP) from channel 1 to the other channels and get it to work correctly.
10. The challenge is to get the other channels after the first to layout correctly on the PCB.
My experience has been that the the ALP does not work correctly no matter what set of components or components and tracks is chosen. Components are left out, and/or components from other channels are included in groups, and/or tracks are left out --- it seems random. It also seems to be dependent but not strictly whether components (and tracks/vias?) are included in a selection that is copied to the clipboard before applying the ALP command. I have not found it better to use groups than to use 'currently selected.'
The end result is that I am left to manually do a lot of work in layout of all of the channels. I cannot carefully layout the first channel and apply that to the rest of the channels. In my current case, I have only 12 components in each channel. Given that spacings are critical, the need to manually do a final edit on every channel (WHENEVER A CHANGE IS MADE TO THE FIRST CHANNEL!), is frustrating. If this were a big design it would be intractable.
I have carefully read the other posts on this problem and attempted to apply the guidance. It hasn't worked in my case.
Forging ahead, very slowly, with great frustration,
Dave
|
| Peter Johnson |
Posted - 01 Mar 2010 : 11:25:44
Well, there's no reason according to the code why using the clipboard should work better, but it does. Do also remember to use groups, including everything you want copied in the original group, not just the components. That will give you the best chance of a perfect copy. |
| Iain Wilkie |
Posted - 01 Mar 2010 : 11:07:14
I seem to remember that when you replicate the circuit in the pcb editor, you must copy it to the clipboard in order for the pattern to replicated properly...
Iain |
| dgeorge |
Posted - 01 Mar 2010 : 06:52:24
I confirm many of the problems that Trev has had attempting to make multiple copies of a circuit (such as multiple analog channels of a signal conditioning board!)
The layout pattern tool does not work very well. A 'seemingly' identical set of components will leave out a couple or more out of a dozen and then manual routing has to be done.
I have tried to figure out a way to make a set of components with tracks, vias, etc., into another component with a set of pads for say, Vcc, Vdd, Gnd, In, and Out. Then one layout for that "component" would allow for insertion of a block into a schematic and for automatic layout on the corresponding PCB. But alas, the pad layout editor will not handle tracks or vias so that approach is not possible. I hope that in a future version that his capability will be included -- i.e. make a pcb symbol capable of handling tracks, pads, and vias.
A bit frustrated with repetition,
Dave
|
| tswelectronics |
Posted - 08 Dec 2009 : 11:15:19
Hi again.
Following on from my last message. I have 4 identical circuits in my design. I grouped the first one and applied the above method of selecting the components and applying the generator to them. I did this for the last of the 4 circuits and I just got bad results. I do not know why. Anyway. I grouped each of the 3 previous circuits together to see if using any of these would make a difference and it did not. But after leaving the design, re-selecting the components and trying again I suddenly got really good results for the final circuit. there must be some other factors that help. i did not move any of the groups or edit them. At present I can only think it was in the way I selected the components to be grouped. I deselected some of the nets leading to it. Maybe this is something?
Hoping it helps.
Trev |
| tswelectronics |
Posted - 08 Dec 2009 : 10:49:58
Well an update from my own experiences.
I first group some components together for my pattern generator. If I then try to apply this group pattern to some more components I do get different results depending how on I implement the generator.
If I leave the collection of components I want the pattern generator to work on in the component bin I get maybe 30% success. If I actually go to the schematic and highlight all the components from there and then switch to highlight them in the pcb. I drag them from the component bin onto the main pcb sheet. I keep them selected and now apply the pattern generator to the selected components I get 95% success.
There were only 3 components in the bin that were not part of the design and these components were unique and difficult to confuse with others. So, somehow there is a difference there.
Trev |
| Peter Johnson |
Posted - 27 Nov 2009 : 15:41:18
No, it really is ambiguous topology that causes the problem. A better way to approach it is to use groups, as then you can make sure that the group you''re applying the pattern to has only the required components in it.
The problem with this approach is that if you have a lot of very similar elements, then the groups necessarily become small, so the benefits of applying the pattern in terms of saving work are reduced. However, there's no other method which will be so effective in avoiding ambiguity. |
| tswelectronics |
Posted - 25 Nov 2009 : 09:05:20
Hi, thanks for the information. I think we might be getting to some interesting points and maybe able to figure out how to work around them.
So, for the decoupling capacitors as your example. It does make sense that is difficult for this. I suppose the pattern tool works off the netlists? So lets say I have 4 identical circuits in the schematic. Would it help to put each of them in a seperate schematic sheets?
Would it help any to have the components numerically labelled close to each other. So resistors, R1 - R20 would be in the first pattern. If I had a second copy of the circuit and ensured the parts were labelled R21 - R40, would this help the pattern generator any?
Thanks for providing a bit of information on the pattern generator. Are there other scenarios the generator has trouble with that we might find 'good practices' for that will help it to work better?
Thanks
Trev
|
| DavidM |
Posted - 25 Nov 2009 : 08:10:33
You are correct, as its name suggests it uses the original arrangement of components and tracks as a 'pattern'. It matches that by component name and connectivity to the selected set to which you want to apply that pattern, and arranges that set to match.
Whilst it will get a complete match in most situations, there are circumstances where it has to make an arbitrary choice between components that are basically identical, which can mean that the result is not laid out in the exact same 'order' as the corresponding set of components in the schematic.
The usual example of this is where you have a number of identical bypass capacitors, as they are all the same component and value and are connected to the same nets, it isn't possible for the pcb function to know that C23 is supposed to be alongside U12 and C24 belongs with U13. The resulting arrangement will be electrically correct, it just won't be in quite the same order as the schematic.
|
| tswelectronics |
Posted - 21 Nov 2009 : 01:19:00
Hi.
Reading your last email, are you saying that the pattern generator is more of a tool that will only attempt to recreate. There is no real gaurantee that it will work?
Trev |
| Peter Johnson |
Posted - 19 Nov 2009 : 10:39:32
In theory you would expect that copying the master in schematic and pcb would work, and as far as named nets go, it does. The problem arises with auto-numbered nets, which just use the next available number.
The chances of those matching is vanishingly small, so when you forward changes, instead of renaming, the nets are deleted and reinstated unrouted. Applying the pattern will restore the tracking.
Bearing in mind that we can see the data, but as for a computer it's just a pattern of interconnects, it is possible for it to get it wrong when the pattern is ambiguous. The simplest case (obviously) is two resistors in parallel, but the one's reported are usually a more complex version of the same issue when the topology is untangled.
From a programming point of view, the problem is not resolving the ambiguity, but actually recognising that there is one in the first case. Doing a comprehensive check in every case would be extremely resource hungry. |
| tswelectronics |
Posted - 17 Nov 2009 : 14:00:40
Thanks for the reply. Copying the master in schmetic and pcb first. Does that not get rid of the need for the pattern layout tool?
I sometimes find it places the wrong resistor in the correct position. And sometimes it just does not find a match for some of the components. So I get left with half a pattern.
Next time it happens I shall send in the files to support.
Trev |
| DavidM |
Posted - 16 Nov 2009 : 12:16:22
...and of course if you have specific examples that show the kind of problems you are talking about, we're always happy to take a look if you can send the data and full description to support. |
| Peter Johnson |
Posted - 16 Nov 2009 : 11:53:52
We've had a number of reports that if you use <Ctrl+C> to copy the master to the clipboard, then apply it from the clipboard it seems to work better, but it's unclear just why this should be so.
The algorithm does sometimes get it wrong, but if you copy and paste the master first in schematic(s) and pcb, then forward design changes, the tracks will unroute, but the components will already be in the right place. That also helps, as there's less potential ambiguity about the netlist. |
