Note that easyeda has two kinds of prefix.  Most components have a label, like R1, C2, D3, U4, etc.  Easyeda calls this a prefix.  The other kind of prefix is the prefix used when placing a module.  Do not confuse the component prefix with the module prefix. Easyeda uses the module prefix to change component prefixes and IDs.  New component prefix = module prefix + old component prefix.  For example, if the old component prefix is R1, and the module prefix is A, then the new component prefix is AR1.  If you use the same module prefix for both the schematic module and the pcb module, then easyeda will change both the same, and the schematic and the pcb will match.  Use a different prefix for each module, and for each copy of a module, but use the same prefix for matching schematic and pcb modules.  For the module prefix, easyeda allows capital english letters, but not numbers, punctuation, or lowercase letters. Once you have placed a pcb module, you cannot move the pcb module.  If you select everything in the module by dragging a rectangle around the pcb module with the mouse, create a group, then move the group, only some of the things in the module will move.  So you should try to place the pcb module in the correct place the first time. If you need to move a pcb module after the pcb module has been placed, select every part of the pcb module, cut, and then paste in the new location.  Or delete every part of the pcb module and place the module again. You can rotate a pcb module 90 degrees by selecting every part of the pcb module, then format -> rotate left/right.  If you want to rotate a module by an amount other than 90 degrees, you might need to open the project which the module was created from, rotate each component in the pcb, then save as a new module. If a pcb module has a board outline, and you place the pcb module into another circuit board, you will have two board outlines.  If you place many modules, you will have many board outlines.  A circuit board should only have one board outline, so you need to delete the extra board outlines.  You can eliminate the work of deleting the extra board outlines by making modules without board outlines.  However, I find the board outlines are useful as guides for placing the pcb modules in the correct locations, so I suggest that modules should have board outlines. If you are placing many pcb modules, and are not sure how to arrange them: Place every pcb module.  Make sure there is empty space around each pcb module, because that makes it easier to select every part of a pcb module without selecting nearby parts.  Make sure each pcb module has a board outline which is the exact shape of the pcb module.  Hide all layers except the board outlines.  Move the board outlines to an empty part of the workspace and experiment with different arrangements.  When you are satisfied with the module layout, make all layers visible again.  Select all components in one module.  Cut.  Zoom and move the workspace until the board outline which marks the correct location for that module is on screen and is large.  Paste the module in the center of the board outline.  Repeat for every module.  When every module is in the correct location, hide all layers except board outline.  Delete every board outline.  Make all layers visible. Create one new board outline. When placing a module with the mouse, the mouse pointer might be far from the module.  If you zoom in so the module fills the display, the mouse pointer might be off screen.  This occurs when the 0,0 origin point of the module project which the modules were made from is far from the image.  This applies to both schematic modules and pcb modules.  I think it is easier to place modules if the mouse pointer is in the middle of the module image. When you make the module project, before you make the modules from the project, move the origin to the middle of the image.  With module project open in editor, place -> set canvas origin, and click the mouse in the center of the image.  Do this twice, once for the schematic and once for the pcb. A pcb module should not have a copper ground plane.  When making a project which will be used to make modules, do not fill unused space with a copper ground plane.  You might need some of the unused space to place tracks connecting the module to other things.  Filling unused space with a ground plane is a good idea, but do not do it until after you have done everything else, after the module has been placed in another circuit board. When you place modules in a project, easyeda renames some of the nets.  Nets are a group of pins, pads, and circuit board traces which are connected. Easyeda renames the nets without labels, but does not rename the nets with labels.  Easyeda expects to connect nets with the same name together, so this means that easyeda expects a net in a module which does not have a label will not connect to anything outside the module.  Easyeda expects that a net in a module with a label will connect to nets outside the module with the same name.  VCC and GND are net labels, so easyeda will expect to connect VCC and GND of a module to VCC and GND of other parts of the circuit.  So when you create a module, you should make sure that any net in the module which will connect to nets outside the module has a label, and that any net in the module which does not connect to anything outside the module does not have a label. If you place more than one copy of a module, there might be some nets you want to connect to something outside the module, but do not want the modules connected to each other.  For example, the module might have a data net that you want to connect to an input/output pin of a microcontroller, but you want each copy of the module to connect to a different input/output pin.  If you label the net, easyeda will try to connect the data nets of every copy of the module together.  If you do not label the data net, easyeda will not try to connect the data nets to anything.  Either way it will be wrong.  I suggest giving the microcontroller input-output pins net labels like GPIO1, GPIO2\, etc; then give the module data net a label like CONNECT\_TO\_MCU\_GPIO\. After placing the microcontroller module and multiple copies of the data module in a new project, edit the schematic and rename the first module data net to GPIO1, rename the second module data net to GPIO2, etc.  Then update pcb, and easyeda should rename the nets on the pcb to match the schematic, and then easyeda will try to connect the nets correctly. It is not possible to place a pcb module until after the pcb has been created.  If you place a schematic module, then create the pcb, then place a pcb module, there will be duplicate components on the pcb, because the components in the schematic are added to the pcb when you create the pcb, then added again when you place the pcb module.  The duplicate components must be deleted.  It is usually easy to delete the duplicate components by selecting many at once by using the mouse to drag a box around the components which you want to delete.  Or you can save a little work by avoiding situations where easyeda creates duplicate components, by creating the pcb before placing schematic modules, and by not updating the pcb until after you have placed the pcb modules. I tried creating a blank pcb from a blank schematic, at the beginning of a project, before placing schematic modules, but easyeda did not allow that. I suggest start with a blank schematic.  Place one schematic module.  Use the simplest module.  Create pcb.  On the pcb, delete everything.  Place the pcb module.  After this, when you place a schematic module, immediately place the matching pcb module.  Do not update the pcb in the middle of placing the modules, after placing the schematic module and before placing the pcb module.

When you place a pcb module, easyeda renames the nets for pins of components, but not the nets for tracks.  This results in mismatches between the tracks nets and the pin nets.  Easyeda marks these mismatches as errors. When you update the pcb, there is a checkbox to rename the nets for tracks, which should fix the mismatches.  So you have to update the pcb after placing pcb modules so that the track nets will be named correctly.  And easyeda will not let you update the pcb unless you have changed the schematic.  So you have to make some change to the schematic in order to update the pcb in order to fix the net names after placing a pcb module. For example, place schematic module, place pcb module, go back to schematic, make connections between schematic module and other parts of the circuit, update pcb. Sometimes when you update pcb, easyeda deletes components from modules and recreates the components somewhere else.  This occurred frequently with older versions of easyeda, less frequently with the current version, and hopefully will be less frequent in future versions.  After doing update pcb, check the pcb for errors.  If update pcb caused errors, undo or revert to a previous save.  Do not keep editing a corrupted file.  One time update pcb corrupted my pcb.  I did undo, then tried update pcb again, but easyeda corrupted my pcb again.  I exited easyeda without saving and restarted easyeda, and then update pcb worked correctly.  This is annoying, but it is not a big problem as long as you save frequently, and do not keep editing a corrupted file.  Always check for errors after doing update pcb, because if you do not realize the file is corrupted, you will lose all the work you did after the file became corrupted. If a pcb module component ID is different from the schematic module component ID, then when you update the pcb or import changes from the schematic, the component will be deleted from the pcb and recreated in a different place, and then will have to be moved to the correct place.  If the component IDs do not match, but you want to change them so they do match, first make sure the prefixes (U1,R2,C3,etc) are the same, then do design -> reset component unique ID, for both the schematic and the pcb. In easyeda, all modules are private in the sense that only you can place your personal modules in a project.  But all modules are public in the sense that anyone can search any modules from any user.  You can go to [https://easyeda.com/search](https://easyeda.com/search), enter a search term, and click on modules; and it will show any module by any user which matches the search term. Schematic modules and pcb modules are mixed together, and it does not show which pcb module goes with which schematic module.  You can select any module.  But you cannot place the module in a project.  You can open the module in editor, then save as module, and you have a new personal module which is exactly the same as the original module.  You can place your new personal module in a project.  Your new personal module is also shared with all other users, even though your new personal module is exactly the same the original module which is also shared with all users.  So if a module is used by more than one user, then search results will include duplicates because there is one copy for each user. If you use a module which is used by other people, then maybe delete your personal copy after you are done to reduce the number of duplicates in module search results. If you have useless personal modules, these are being shared with other users and are messing up other people's module search results. Please delete your useless modules. To delete a schematic module, start the editor, do library, EasyEDA, SCH Module; select the module, click More, click delete. Delete pcb modules the same way except PCB Module instead of SCH Module. If you place a module in a project, then edit the module, then want to update the project to include the changes to the module; then I think easyeda does not have a way to do that, other than deleting the module components and placing the module again. One way to link matched schematic and pcb modules together is to give both the same name.  Easyeda keeps schematic modules seperate from pcb modules, so it is not a conflict if a schematic module and a pcb module have the same name.  I suggest using names which are a short description.  There is no need to put module, schematic, or pcb in the name because easyeda already remembers these properties. When you save a project as a module, there is a place in the save as module dialog box to enter a description.  Modules do not inherit the description from the project.  Module descriptions are not shown when a user is searching for modules.  Module descriptions are shown when a user is listing modules in the personal library, but only in a small space, so the description should be short.  I use a short description as the module name. Repeating this information in the description is redundant, so I leave the description blank. Another way to link matched schematic and pcb modules together is to get the URL of the project which the modules are saved from, and put the URL as a text comment in the schematic.  This text comment will become part of the schematic module, so anyone looking at the schematic module will know how to find the project which the module was created from.  Then put the URLs of both modules in the description of the project.  You could put the URL of the pcb module in the schematic module, but you need to make the pcb module first, then put the URL in the schematic, then make the schematic module. You could put the URL of in the pcb, but it would probably need to be deleted when placing the pcb module in a project. Modules do not inherit the attachments of the parent project.  Easyeda does not allow modules to have attachments. Easyeda does not have a way to link documentation to modules.  You can attach documentation to the project which the modules were saved from, and include the URL to the project in the schematic module. You can post the documentation in the easyeda forum with the URL of the modules. You can create a web page outside easyeda with the modules and documentation. I tried to create a set of modules which are compatible with each other, consisting of a microcontroller module plus input-output circuit modules. These modules could be used to create many different circuit boards by using combinations of input-output circuits.  Easyeda has no way to link the modules together as a set of compatible modules, so you have to know and remember which modules are compatible with which other modules. This information was correct for the web version of easyeda in december 2021.  This information might not be correct for the downloadable version of easyeda, or for future versions of easyeda.

@kenneth_howlett, Thanks for your detailed description of how to use modules. You might like to copy and paste the text from these posts into the Description section of a public EasyEDA Project and then post a link to it here in your (edited)  first post in this topic. That way, you can easily edit the text if you wish to keep it up to date and you could include some examples to help illustrate some of the points in your How To.

You might also like to have a look at this topic: [https://easyeda\.com/forum/topic/How\_to\_use\_Modules\-8CbnXVvsq](https://easyeda.com/forum/topic/How_to_use_Modules-8CbnXVvsq)<br> <br> and: [EasyEDA-Tools](https://github.com/ppeetteerrs/EasyEDA-Tools) by Peter Yuen [easyeda-MyExtensions](https://github.com/duritskiy/easyeda-MyExtensions) by duritskiy in: [https://easyeda.com/forum/topic/Extension-User-Extensions-for-EasyEDA-Summary-9e065b68316f4491a3911dc6204be31e](https://easyeda.com/forum/topic/Extension-User-Extensions-for-EasyEDA-Summary-9e065b68316f4491a3911dc6204be31e)

Here is a tutorial video on how to make and work with modules in EASYEDA [https://youtu.be/E2dszWjxtAY](https://youtu.be/E2dszWjxtAY)