Connector Library > Conn_02x04_Counter_Clockwise should do the trick for the Symbol, then match to a DIP-8 footprint.
Don’t forget @Lawrence_Joy , the IC is now not part of the Schematic or PCB. The IC is just something or other that you can fit into the socket.
My modus operandi is to use the IC symbol but to assign the socket footprint to it. That way I get the board rendered correctly in 3D. If I want to see the IC in the socket I add its 3D model, displaced a bit in the Z dimension.
The problem with this is that the BoM is wrong for assembly because it’ll have the IC but not the socket. But since I assemble by reaching into my BoJ (Box of Junk) I’m ok with this BoJ, er, bodge. 
Not me. I only use DIP sockets for repair if I have to.
But if you are looking in the lib “Socket”, you will miss 8 pin sockets.
Also, I’m only explaining how this happened and not complaining about missing DIP-8 footprints.
Ok, I won’t socket to you then. 
Okay folks, In the footprint editor I did find sockets, even a DIP-8 socket that I can use. However, when I go to “Assign Footprints” it lists the parts by reference designators and so there is no XAR1 ref des as of now. So I placed another LM386 IC on the schematic, changed the ref des from U? to XAR1, went to “Assign Footprints” and assigned the DIP-8 socket. Now on the schematic how do I render the graphic symbol invisible, just leaving the ref des to move around and place by the AR1 ref des? Or do you have other steps to follow to accomplish this? Thank you.
Need this adding to the Forum . . .
Your workflow is very strange. Why does the refdes have to be XAR1? Can’t you just use U? since it’s a LM386 IC? Why do you want to make the U? symbol disappear and put it by the AR1 (I thought it was XAR1?) symbol? Then you have two symbols to assign footprints to, no?
If you can you shoud post your project otherwise you’re just digging yourself deeper and deeper into a workflow that only makes sense to you.
Be patient! The LM386 is an audio-amplifier. Next month he will ask what he could do how to name the second LM386 as he decided for a stereo amp. And where to find left channel DIP-8 footprints.
Okay, ha ha. Let’s do this another way. How do I enter onto the schematic the graphic symbol for an IC socket? In this case the graphic symbol for an 8-pin DIP socket? As I have not been able to find a graphic symbol in any of the symbol libraries I guess I would have to make one myself. For the ref des class letter X, this is for a socket; a fuse holder or fuse clip(s), a lamp holder, even a battery holder. Putting the X as a prefix to a base part ref des this indicates it’s a socket for the base part. So XAR1 means it is a socket for AR1. I’ll go off and try my idea and get back with you when I get it figured out. Thanks in the meantime for all your replies.
Just draw a graphic box around the IC if you really have to. But this works only if the IC has only a single unit (other than power). Otherwise you end up twisting the schematic to fit all the units in the box. Similar to those people who draw split vacuum tubes because they think the schematic should resemble the physical entity. Actually this was common in early schematics containing ICs, the draughtspeople couldn’t get used to the idea that the schematic was an abstract representation. And those people who insist on making the symbol look like the IC package because they come from Fritzing or similar.
The schematic is a just a abstract representation of the circuit. You can add graphics and text to document other aspects.
Here are some possible arrangements:
Use the IC symbol but make the footprint that of the socket. 3D rendering is correct, but the BoM is wrong because it contains the IC instead of the socket.
As above, but change the value of the symbol to be the part number of the socket, so the assembler knows. The IC you have to fit yourself, or write a note to the assembler to fit.
If you are assembling this yourself, then make notes on the schematic so you remember what to do.
Don’t know why you need the complication with (X)AR1 and IEEE clauses. Sounds like you overthunk it.
Edit: For my hobby efforts, I don’t bother to represent IC sockets. I just decide to use them or not for a given board, e.g. I may use sockets for the testing board, then remove the ICs and solder them on a “product” board.
For a part in a socket I always used two parts in the schematic. The normal schematic graphic representation (U1 for example) and a socket *SKT1". I always avoided sockets as I do not feel they are as reliable as soldered in parts. It was also very common to see ICs pushed into sockets where a pin was bent up under the part, impossible to see. Worse yet the bent under lead could be touching the socket metal which got a board through test only to die later after being shipped.
One of the schematic parts (typically the U1 part) was fed to the BOM while the SKT is feed to PCB design.
Bob K.
Maybe this, and linked topics there are of some help: Duplication of PADs for symbols.
I have a feeling that we receive quite many questions which look very different but in the end boil down to two or three basic things:
But the third point comes only after the fist two.
[SOLVED!] alright all you yahoo (derogatory meaning) people. Like the comedic magician said, “I’m going to show you this trick without using strings, wires, or lubricants; nothing up this sleeve, nothing up this other sleeve”:
• Place on the schematic the through hole part you want to use. Disassociate any footprint. Assign ref des such as U3.
• Place on the schematic the graphic symbol for the socket you want to use. You may have to modify the socket symbol from male (pins) to female (sockets). Assign ref des such as XU3.
• Place connection lines from circuitry to the socket terminals coinciding with the part terminals.
• Attach footprint of socket.
You are now done and have two parts that will show up in the parts list (PL). KiCad will throw errors when doing an ERC indicating that your original part (U3) is not connected. You know this and can live with it because the connections are to the socket. If you don’t want to use the socket, produce a 2nd PL with DNI (do not install) or DNP (do not populate) for the socket(s). Ta-DA.
Here is another scenario that you are more likely to run across. You have a fuse that you want to attach to a PCB using a couple of fuse clips:
• Place a fuse symbol on the schematic–no footprint. Assign ref des such as F1.
• Place two fuse clips on the schematic with footprints. Under the Unit Numbering method of assigning ref des these fuse clips would be assigned ref des of XF1A and XF1B. However, because KiCad does not understand suffix letters used with individual parts, use XF1E1 and XF1E2 (in this case the class letter E stands for miscellaneous electrical part or a terminal).
• Show connecting lines on the schematic to the fuse clips. Again the fuse is just hanging out there in space and the PL will list all three parts, and therefore, all parts are accounted for.
• Your done. What more do you need?
Thanks for reading.
Thats easy to fix . . . mark all pins as not connected.
Ah yes, thanks about the reminder of use of the “No connect flag”.
FWIW, I’ve now standardised on the opposite:
So DRC/ERC is happy, the BOM is accurate, the 3D models are well associated, and assembly is bit more logical (the socket is populated at soldering time, and the pluggable then can be plugged in at the same time as other post-soldering mechanical things).
PS. I’m less interested in all the designator rules.
Well it’s not the total opposite, the only difference is that you use the socket rather than the IC symbol. The drawback with that is you don’t get to reuse the symbol for the IC that has already been developed and the pin types. Also it doesn’t work with multi unit ICs. But it’s only a matter of which tweaks one is willing to do to make things fit into the KiCad scheme.
Yes, it’s subtle and tweaky.
One subtlety that might not be apparent: it is the IC symbol. Multi-unit and all. I just change the fields so the ordered item is the socket, and the footprint is the socket.
So in the screenshot, A1 is the standard Arduino symbol, but I fill out the fields so on the BOM you’re ordering the headers. Then I tweak the footprint so it’s just the headers, and move the actual Arduino content to the new H1 symbol.
That’s how I described it so we are in furious agreement.
Oh, so we are! I appear to have furiously misread.
