Hi Biophob! Is the current supposed to flow towards JP1(pin9&10) with D1? If that is the case, then your diode D1 is wrong way around in schematic, which means that D2 is also wrong way around. You have dual power supply. positive rail should be connected from anode to cathode going towards JP1. Negative rail should be connected from cathode to anode going towards JP1 assuming that JP1 is power output connector. Regards, Markus Virtanen HW / Electronics Designer

Thank you for response. No, the JP1 supplies the device. It is dual supply with positive and negative voltages. But what I mean is the symbol of the diode is reversed on PCB compared to schematic. Here is example how it should look like and how it looks currently. The marking bar on a diode switched sides. Am i doing something wrong? 

And the schematic is OK.

Select the Schematic Symbol for the device then click on the Footprint (a.k.a. package) attribute in the right hand panel. This will show you the pin mapping. Edit the symbol pin or the footprint pad numbering so that the symbol pins map onto the footprint pads in the correct order or orientation. Then click Update. Then close the Footprint Manager. If you use the right click Find Similar Objects... tool then you can select and edit all the diodes at once.

Thank you @andyfierman, but it didn't change the orientation of diodes on PCB. Would be great to elliminate the cause of the disorder, not just the effect. It can make big problems. I don't get it, why is it happening? I'm lucky I have spotted this one.

@Biophob, Have you done **Update PCB...** or **Import Changes...** to pull the changes in the Schematic into the PCB?

"I'm lucky I have spotted this one." Not quite. Strictly, you should have found and corrected this error before you did **Convert to PCB...**. This is what the Essential Checklists (4) and (6) are for in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a)

This is nuts! What is happening? It looks like it treats the diode pinouts randomly! How to prevent it? Does it happen only for 2-pin elements? Or do I have to check EVERY COMPONENT i use? Even the ones with 3 pins or more? I dont have pinouts of every existing component in my head to check it every time. Besides, i have not found (4) or (6) in your link. It does not contain the words "essential" or "checklist" so I'm assuming you put the wrong link. 

@Biophob, Have you done the steps described above? * _Select the Schematic Symbol for the device then click on the Footprint (a.k.a. package) attribute in the right hand panel._ * _This will show you the pin mapping._ * _Edit the symbol pin or the footprint pad numbering so that the symbol pins map onto the footprint pads in the correct order or orientation._ * _Then click Update._ * _Then close the Footprint Manager._ * _If you use the right click Find Similar Objects... tool then you can select and edit all the diodes at once._ "Besides, i have not found (4) or (6) in your link. It does not contain the words "essential" or "checklist" so I'm assuming you put the wrong link." You have misread the instructions: _This is what the Essential Checklists (4) and (6) are for in (2) in:_ [_https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a_](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) You open the doucment in the link then you read it at least until you get to and open the link in this bit:  then you find: 

If you are using User Contributed parts then you **must** check them.

@Biophob I do suggest using LCSC part numbers. That way you can be pretty sure that the cathodes and anodes are in the correct way. Using user contributed parts is always a risk if you don't check the component footprint.  Regards, Markus Virtanen HW / Electronics Designer

All components were from the System library. And all of the diodes in the screen i put above. Sorry, I did not expect link inception. Scarcely your screen has an answer. Editing in Footprint Manager didn't swap the diode pinouts. Now i'm trying to find properly oriented diodes. I can't believe it. Thanks for your help. I am going to report all diodes with false footprints.

This part in the System library is wrong:  If you find a mistake in **any** part please submit an error report about it clearly stating what is wrong and what action needs to be taken to correct the error using the **Report Error** menu option:   Please note that I have submitted this report.

@Biophob, Hmmm, I'm not suprised that you're confused. It looks to me like the Footprint Manager is broken. Please see: [https://easyeda.com/forum/topic/Pin-numbers-but-not-pin-names-can-be-corrected-in-the-Footprint-Manager-7b2d4c883e0249639722c68db2263556](https://easyeda.com/forum/topic/Pin-numbers-but-not-pin-names-can-be-corrected-in-the-Footprint-Manager-7b2d4c883e0249639722c68db2263556)

Hi All It fixed now. we re-assign a footprint for it. and at LCSC classe has a PMLL4148L,115， it is correct, suggest using LCSC part first. Thank you for report. 

I would like to give a bump to this topic. Even when using only LCSC contributed Footprints, the diodes are an absolute NIGHTMARE! Their orientation \(pin 1 or 2 at anode\) is completely inconsistent and in fact most of them link the default diode schematic symbol \*the wrong way around\*\. I know that such stuff has to be double checked, an I do. But for new users this situation should be improved. When someone drops e.g. a LED from the library into their schematic and then changes footprints from 0603 to 0402, and they end up the wrong way in the board this is not userfriendly..

Moreover\, swapping the pinouts of many parts via the footprint manager \*DOES NOT WORK\*\. When selecting a bunch of wrongly assigned diodes\, reversing the pinout\, and updating\, the changes will be applied only to one of the diodes\.

@tobalt, Hmmm. I raised a Bug Report about this over a year ago. Please repost your comments about batch updating not working in the Footprint Manager as a reply in this topic: [https://easyeda.com/forum/topic/Footprint-manager-Batch-Update-not-working-364a249cbeee47bfa9883cfe43b02a1f](https://easyeda.com/forum/topic/Footprint-manager-Batch-Update-not-working-364a249cbeee47bfa9883cfe43b02a1f)

@tobalt, Please also add some screenshots to illustrate the issue. Thanks.

I drop a 0603 LED:  Alright, its footprint is fine:  But now I want it to be a 0402 LED (there are no 0402 LEDs in the quick menu EELib). So I type 0402 in the search in filter for LSCS footprints since these should be quality controlled I suppose.  Surprise, it is the wrong way around. What's more: about half of the 0402 footprints are the proper way, half of them are wrong.. And it has nothing to do with the "R" in the name. It is just random...

The problem here is that you are trying to use a symbol for one part and the footprint for another, different part. In an ideal world all component symbol pin to footprint pad mappings would be consistent. So all diodes would have anode as pin 1 mapped to the anode end pad of the footprint and cathode pin 2 mapped to the cathode end pad of the footprint and that would be the same for every diode from any library. And that consistency would apply to every component in every library. Sadly for a number of reasons, it does not. Instead of placing a generic part from the EELib and then replacing the footprint for it with one for a different part in another library, if you replace the symbol in the schematic with the one for the desired new part and then do Update PCB..., that should pull in the footprint with the pin mapping already correct to the symbol in the schematic. If you still find that the pin mapping is wrong because whoever created the symbol made a mistake when creating or assigning the footprint to it then please submit an error report using the Report Error tool (right-click the selected part in the Libraries tool).