Consistency errors

On 8/31/2016 12:00 PM, Jim McAuley wrote:

Well, its happened again. I have consistency errors. How do I resolve them. I have tried to delete the offending part from the schematic, both with the board open and closed. I have tried replacing the offending part with a new part from a brand new library. I have tried to delete the part from the schematic, close the schematic reopen the schematic and the board. I have airwires on the board but can't place or select the part. What do I try next?

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/204818

 

Hi Jim,

I hope you're doing well. Remember to always have the board and

schematic open at the same time together. That will avoid running into

consistency issues.

Remember to run the ERC often as you make changes to make sure you are

going the right direction. When you are trying to get back consistency

you need both the schematic and the board to be open at the same time.

How many errors do you have now? If the error is part is found in one

editor but not the other. Then the easiest thing to do is to remove the

part from the editor that has it.

Remember that ALL of the consistency errors must be resolved before you

can regain consistency and continue working.

hth,

Jorge Garcia

I currently have 3 errors and two warnings, all on the schematic.

The errors are "Different connections on Pins" on two different parts.

The warnings are "Only one pin on net" for two different nets.

What do I do to correct these errors, and will this get me back consistency?

Jim McAuley wrote:

 

What do I do to correct these errors, and will this get me back consistency?

Change the schematic so the connections in the schematic match the connections in the board. Make the changes one at a time and run ERC after each change to see if the error has gone away. If it hasn't gone away then the change wasn't right. Once you have made all the changes and got back consistency, you can make the changes in the schematic again to get it to how you really want it to be but remember NEVER EVER edit the schematic or board without the other one being open.

Best Regards,

Rachael

I can't make the connections match between the two. Among the many problems I have is:

1. one of the parts on the schematic won't connect to wires drawn on the schematic unless I press the ALT button.

2. In trying to resolve Drill Distance errors, which got this mess started, I created a new library for the original part, new symbol, new package, new device. In doing this, the schematic was closed as was the board. Upon reopening the schematic and updating the library, I got the consistency error. Now, if I add the missing part to the board it is entered as E$1, the schematic is showing U$1. I cannot change this lable, I cannot move this part, I cannot check info on the part, I cannot select this part in anyway except via the command line. This also means that I cannot make connections to a part that is no longer recognized by eagle board editor.

3. I had already completed routing the entire board, and was in the process of resolving 4 drill dimension errors and 16 overlap errors on this same part. Thats why I recreated the library. The new library had 16 clearence errors that I think I have corrected, but can't check because I have consistency errors.

Should I just delete the board and lose 1 months worth of work or does anyone have any other ideas?

How do you delete the board.

Jim McAuley wrote:

 

I can't make the connections match between the two. Among the many problems I have is:

1. one of the parts on the schematic won't connect to wires drawn on the schematic unless I press the ALT button.

Do the nets in the schematic have different net names to those in the board?

Jim McAuley wrote:

 

2. In trying to resolve Drill Distance errors, which got this mess started, I created a new library for the original part, new symbol, new package, new device. In doing this, the schematic was closed as was the board. Upon reopening the schematic and updating the library, I got the consistency error. Now, if I add the missing part to the board it is entered as E$1, the schematic is showing U$1. I cannot change this lable, I cannot move this part, I cannot check info on the part, I cannot select this part in anyway except via the command line. This also means that I cannot make connections to a part that is no longer recognized by eagle board editor.

Have you updated the part in both the schematic and the board with the new library part?

Jim McAuley wrote:

 

3. I had already completed routing the entire board, and was in the process of resolving 4 drill dimension errors and 16 overlap errors on this same part. Thats why I recreated the library. The new library had 16 clearence errors that I think I have corrected, but can't check because I have consistency errors.

Should I just delete the board and lose 1 months worth of work or does anyone have any other ideas?

 

No you shouldn't delete the board. 3 errors (ignore the warnings they are not important at this point) is nothing and absolutely no reason to delete the board and lose a month of work.

Best Regards,

Rachael

On 31.08.2016 21:35, Jim McAuley wrote:

I can't make the connections match between the two. Among the many problems I have is:

1. one of the parts on the schematic won't connect to wires drawn on the schematic unless I press the ALT button.

Sounds like your schematic and/or lib part was drawn off 0.1inch grid.

This is not recommended, cause schematic doesnt catch pins, like a pcb

does with pads. But I dont understand how that could have happened.

2. In trying to resolve Drill Distance errors, which got this mess started, I created a new library for the original part, new symbol, new package, new device. In doing this, the schematic was closed as was the board. Upon reopening the schematic and updating the library, I got the consistency error. Now, if I add the missing part to the board it is entered as E$1, the schematic is showing U$1. I cannot change this lable, I cannot move this part, I cannot check info on the part, I cannot select this part in anyway except via the command line. This also means that I cannot make connections to a part that is no longer recognized by eagle board editor.

You can rename E$1 and U$1 to the same new name and you are one step

closer to consistancy. You need to practice a couple of new functions

that you normally dont do on board, when consistant. That is the name

and net functions. Net connects pads with airwires, and it needs to be

connected as on schematics. Also name the airwire to the same netname as

in schematics. Do ERC after every change to see how it went.

When this is said, I myself found a lost consistancy a few days ago

(with 7.6.2 bet), so I know there are some rare bugs left. But since I

was unable to focus on repeating it, I just fixed it and let it pass for

this time.

3. I had already completed routing the entire board, and was in the process of resolving 4 drill dimension errors and 16 overlap errors on this same part. Thats why I recreated the library. The new library had 16 clearence errors that I think I have corrected, but can't check because I have consistency errors.

 

Should I just delete the board and lose 1 months worth of work or does anyone have any other ideas?

No! Thats a waste of time. Use this event to learn how to regain

consistancy. Once you know howto, its not that hard.

PS:

Eagle always keeps the last 10 backups, named .s#1 for the last, .s#2

for 2nd gen and so on. For boards, the name is .b#1,... You can try

recovering you data there. Check their creation date and rename the

chosen ones to .sch and .brd (may be worth backing up the bad files).

On 31.08.2016 21:35, Jim McAuley wrote:

I can't make the connections match between the two. Among the many problems I have is:

1. one of the parts on the schematic won't connect to wires drawn on the schematic unless I press the ALT button.

Sounds like your schematic and/or lib part was drawn off 0.1inch grid.

This is not recommended, cause schematic doesnt catch pins, like a pcb

does with pads. But I dont understand how that could have happened.

2. In trying to resolve Drill Distance errors, which got this mess started, I created a new library for the original part, new symbol, new package, new device. In doing this, the schematic was closed as was the board. Upon reopening the schematic and updating the library, I got the consistency error. Now, if I add the missing part to the board it is entered as E$1, the schematic is showing U$1. I cannot change this lable, I cannot move this part, I cannot check info on the part, I cannot select this part in anyway except via the command line. This also means that I cannot make connections to a part that is no longer recognized by eagle board editor.

You can rename E$1 and U$1 to the same new name and you are one step

closer to consistancy. You need to practice a couple of new functions

that you normally dont do on board, when consistant. That is the name

and net functions. Net connects pads with airwires, and it needs to be

connected as on schematics. Also name the airwire to the same netname as

in schematics. Do ERC after every change to see how it went.

When this is said, I myself found a lost consistancy a few days ago

(with 7.6.2 bet), so I know there are some rare bugs left. But since I

was unable to focus on repeating it, I just fixed it and let it pass for

this time.

3. I had already completed routing the entire board, and was in the process of resolving 4 drill dimension errors and 16 overlap errors on this same part. Thats why I recreated the library. The new library had 16 clearence errors that I think I have corrected, but can't check because I have consistency errors.

 

Should I just delete the board and lose 1 months worth of work or does anyone have any other ideas?

No! Thats a waste of time. Use this event to learn how to regain

consistancy. Once you know howto, its not that hard.

PS:

Eagle always keeps the last 10 backups, named .s#1 for the last, .s#2

for 2nd gen and so on. For boards, the name is .b#1,... You can try

recovering you data there. Check their creation date and rename the

chosen ones to .sch and .brd (may be worth backing up the bad files).

On 01.09.2016 09:46, Morten Leikvoll wrote:

that you normally dont do on board, when consistant. That is the name

and net functions. Net connects pads with airwires, and it needs to be

Correction.. I mean the "signal" function, not the net. The signal

creates a net (I bet I did that name mistake at least once before)

On 01.09.2016 09:46, Morten Leikvoll wrote:

that you normally dont do on board, when consistant. That is the name

and net functions. Net connects pads with airwires, and it needs to be

Correction.. I mean the "signal" function, not the net. The signal

creates a net (I bet I did that name mistake at least once before)