Question on package creation in Eagle.

[Alan0354]

I found the answer, but I don't see the delete post feature here.

 

[Alan0354]

I have new questions:
1)What is silkscreen and solder mask layer called?
2)When I create a device, I notice there is something in tStop and bStop layer that looks like solder mask, what can I do to change the size if it is solder mask, I might want to remove the solder mask completely. Any way to do this in the pad when I create the device?

Thanks

 

[keith1200rs]

Silk screen is 21/25 for top. 23 is needed to enable selection of devices. 27 could be included if you like but it isn't normal to include values. Which ones are actually used depends on what you choose to make the Gerbers. For example, you could use 21 but not 25 to show the outlines but not the component reference (for when there is no room for the reference). 51 is often used as an assembly aid on small surface mount devices.

Solder mask is "Stop" as you have guessed - 29/30. Solder paste is "cream" - 31/32. Most of these are automatically created based on design rules. Design rules also set the oversize for the solder mask. They also set the minimum annulus for inner layer pads.

Quite a few PCB houses supply DRC files for Eagle which are worthwhile using.

I am not sure what you want with your last question. Drawing on layer 29 will create a hole in the solder mask (it is a negative layer). If you want some copper covered in solder mask then it must NOT be a pad as they automatically get a mask. Use a track, rectangle or polygon.

Keith

 

[Alan0354]

Silk screen is 21/25 for top. 23 is needed to enable selection of devices. 27 could be included if you like but it isn't normal to include values. Which ones are actually used depends on what you choose to make the Gerbers. For example, you could use 21 but not 25 to show the outlines but not the component reference (for when there is no room for the reference). 51 is often used as an assembly aid on small surface mount devices.
I saw a video about putting ">NAME" in tNAME layer so it will follow the schematic. What does this mean, I don't even know what is the meaning of "NAME"? I saw the video he wrote the name of the component ( say LM741) in tVALUE layer, that confuses me. Which one give you the reference like U1, U2 etc.?
Solder mask is "Stop" as you have guessed - 29/30. Solder paste is "cream" - 31/32. Most of these are automatically created based on design rules. Design rules also set the oversize for the solder mask. They also set the minimum annulus for inner layer pads.

Quite a few PCB houses supply DRC files for Eagle which are worthwhile using.
What is this, I am not familiar with this.
I am not sure what you want with your last question. Drawing on layer 29 will create a hole in the solder mask (it is a negative layer). If you want some copper covered in solder mask then it must NOT be a pad as they automatically get a mask. Use a track, rectangle or polygon.

Keith

Really appreciate your time to help me.

Regarding to the last question. I want to edit the shape of the default solder mask that comes with the pad automatically when creating the footprint. I notice that when you add a pad, the solder mask comes along. I want to change the size, or I want to eliminate it in some cases. I have not managed to modify the solder mask of the pad in the footprint creation window.

Again, I really appreciate your help.

Alan

 

[keith1200rs]

A pad with no hole in the soldermask isn't a pad - it is copper but you cannot connect to it. That is simply a copper area which you can create as a track, rectangle or polygon. If you then want a solder mask hole of some size you can then draw it on the solder mask layer. Assuming you do want a connection to it, simple add a tiny pad to the polygon.

There may be a way of changing the clearance of individual pads but I doubt it - a lot of those things are set globally in the design rules - I can check tomorrow when I am at a computer.

Keith

- - - Updated - - -

I have just checked and there is the option to turn the soldermask on and off on individual pads in library parts and also the solder paste. Click on "change" when editing a package in library to see what you can do.

Keith

 

[Alan0354]

Thanks, I have more questions:

1) If I create a package with through hole pads, how can I check the pad dimension and drill size once I created it? I know when you create it, you can set the pad diameter and the drill size, but I want to verify later on.

2)After I created the device, I pulled it into a schematic and layout the board. But if I find out I need to change the package in the library, how do I update the schematic and the layout after I make changes in the library? Does the layout save the symbol and package information once you import into the schematic and pcb so even if you change the device in the library, it won't automatically update the pcb and schematic?

3) So I can specify using layer 21 tPLACE as silk screen layer to the pcb house?

4) Don't look like I can type in the pad size or drill size, I have to use whatever the size it is given?

 

[keith1200rs]

I have to answer from memory for now.

1. If you are in the library editor you should be able to 'show' item properties. Type SHOW and click on it. If you turn on 'drills' layer (I think) it will show a different symbol for each size.

2. The part is stored in the schematic/PCB file. If you change the library, select the update library menu option to update the schematic/PCB.

3. Normally it would be 21+25. 21 is for the outlines, 25 for the 'names' = component references.

4. You can overtype the value in the box at the top menu with anything you like. Or type 'drill 0.6' for example. Or 'diam 0.9'.

Keith

 

[Alan0354]

Thanks for the help Keith. I manage to create symbol, package and link them to create the device and pull into schematic already. And I managed to modify the pads and pin per your instruction.

 

[Alan0354]

How do I create symbol of components with multiple devices. Say I need to create quad opamp LM324. It has 4 opamps. I want to create U1a, U1b, U1c and U1d. Each is an opamp symbol.

Also, say if I put a ground plane on the top layer, how do I control what clearance between pads and the ground plane? Is there a way to set the clearance distance?

Thanks

Alan

 

[keith1200rs]

Alan,

Apart from tutorials, the easiest way to find out how to create parts is to look at existing ones such as 4AMP_P4+12 in LINEAR.LIB.

The basic procedure is simply to add more SYMBOLS to the DEVICE. You can also add optional power pins there if you like. Look at the help for information on ADDLEVEL and SWAPLEVEL.

Clearance for polygon fills will be the minimum by the design rules if you set ISOLATE to zero. If you want something larger than the minimum (I usually do) then set ISOLATE to something larger.

I missed a couple of your earlier questions - maybe you have sorted them out now:

>NAME on the NAME layer is replaced by the NAME of a device (and similar for >VALUE). If you just wrote NAME then all parts would be labelled NAME instead of R1, R2, R3 etc.

If you run the DRC there is an option LOAD. That enables you to load a DRU file. You can easily create your own - set the design rules then use the SAVE option. You can also download them such as this one from PCB-Pool http://www.pcb-specification.com/images/stories/Downloads/deu_EAGLE_DRU_Datei_CM0610.zip

Keith.

 

[Alan0354]

Thanks Keith AGAIN for your great help. I did the multiple device already. I have a few more question:

1) I try to save the device under other name, eg. I create a quad op-amp MC33179, I want to create TL064 which is exact same package and symbols except the VALUE that show the name of the component. I try to open the MC33179 and use "SAVE AS", but that become a library. Matter of fact, I have tried to pull a device from another library ( say from Linear.lbr) and put it in my custom library. I cannot manage to do that. Not even having the exact name and package. All I want is to copy a device from one library to another.

2) After I create the symbol and package, when I pull the symbol into schematic and package into pcb, how can I move and rotate the NAME eg. R1, U1 etc. When making the schematic, you rotate the part around, the reference designator need to be rotate and move to a more convenient location. I cannot manage to move them.

Thanks

Alan

 

[keith1200rs]

Alan,

I cannot see the point of having two identical devices with different names - you can simply change the name after placing it.

The simple way to copy devices is to use the control panel. Have your custom library open in the library editor. Browse to the device (or package) you want to copy in the control panel and right click on it. Select "copy to library".

You can copy symbols and packages using cut and paste either within a library or from one library to another but you cannot cut&paste a device.

The procedure may have changed slightly in version 6 - I am still using V5.11.

To rotate names on the PCB (or move or re-size them) you first need to SMASH them. That creates a small cross which allows you to move the name/value separately from the part. The easiest thing to do is simply select the whole PCB and SMASH it all. I cannot see a good reason to not be able to edit/move them.

Keith.

 

[Alan0354]

Thanks Keith. I got stuck with copying parts from one library to another because at the process, it asked whether you want to save as the name of the the destination .lbr. I thought it want to replace the whole library, that's the reason I did not go any further as I don't want to erase the parts already inside the library. But actually it is just simply adding to the library. I made a copy of the library in somewhere else before I copy the part in, everything is ok. Thanks. I always like to put all the parts I use in one custom library so I can easily reference to it.

Yes, I tried group smashing and I got it.

Do you have ways to change the reference and name after smashing. I can move and rotate the reference, but what if I want to change the reference? Say from R1, to R101?

Further more, is there any way to reflow the reference? When I create a schematic and later adding a resistor, the reference number is totally out of place. For example, I create a schematic with 100 resistor, so the next resistor I add will automatically start at R101. But if I add to a part of the circuit that the resistor is from R1 to R10, that R101 is totally out of place. I want to reflow the reference so the number go in progression again.

In OrCad, I can reflow just by one simple command. Any suggestion?


Thanks

Alan

 

[keith1200rs]

You can always manually change any names e.g. R1 to R101 provided it doesn't create a duplicate name.

You will find lots of useful extra commands in the ULPs (click on the ULP button). For schematics, there are things like BOM. For PCBs there are things like CMD-RENUMBER which allows you to renumber the parts on a PCB based on location which I think is what you want. There are dozens of user written ULPs on the Eagle (Cadsoft) web site as well.

Keith.

 

[Alan0354]

Thanks, got it.

I have something puzzling, I pull in parts into the schematic. Later on, I have to modify the part. Yesterday, all I have to do is after modify the part in the library, I go to the schematic page, click Library at the top, click Update and click the name of the library containing the part, all the parts in the schematic will be updated.

BUT tonight, when I do that, the part is not being updated. I have to actually do ADD part to pull in the updated part and delete the old part!!! What is the reason?

 

[keith1200rs]

I have never seen that problem. Have you changed anything in the base name of the part that could make it not recognise it as the same one?

Keith.

 

[Alan0354]

I have never seen that problem. Have you changed anything in the base name of the part that could make it not recognize it as the same one?

Keith.

I found the problem. If you smash the component in the schematic, you cannot update the location of the NAME and VALUE. Smashing does not prohibit the changing of the line changes of the symbol.

Do you know of any ULP that can keep some of the existing reference destinations on the schematic, but refloat the rest of it? In OrCad, all you have to do is change the reference destination from say R10 to R? on the parts that you want to refloat, then run the refloat. The ones that has a true reference destination will remain the same, only the ones laber R? will get new reference number.

I really appreciate all your help.

 

[keith1200rs]

Do you know of any ULP that can keep some of the existing reference destinations on the schematic, but refloat the rest of it?

By "refloat" do you mean physically or numerically? If you select SMASH then hold down the SHIFT key when you click on a component it will UNSMASH it.

In terms of varying some references (NAMES) and not others, I am not sure. Have a look at the ULPs at typing in something like renumber in the search box.

Something such as **broken link removed** may be of interest. or **broken link removed**

Keith

 

[Alan0354]

Thanks Keith.
I finished the schematic and create all the devices. Now I am getting into the layout part. I have a few question as I just started the layout.

1) Is there any way to lock down the component after placing?
2) If I draw a copper plane on the top layer, how do I link the ground signal to the plane.
3) How do I specify the thermals? How to set the size, the spoke width( connection from pad to plane)?
4) Anyway to set nets to different color? Say I want to set the ground net to green and Vcc to red.
5) Can I set the routing width on the net so I don't have to modify every time?

 

[keith1200rs]

1) yes - search for LOCK in the help
2) select POLYGON then before drawing it, type the net name in single quotes e.g. 'GND'. If you have already drawn it you can rename it with NAME.
3) Under the POLYGON help there is a section on THERMALS and ISOLATE. Also you need to look under the DESIGN RULES where some of the thermal rules will be defined such as under the SUPPLY tab. Search for THERMAL in the help and you will find references which are useful under LAYER, PAD and SMD
4) Not that I know if.
5) CLASS might be useful to you, but I don't think it will force a different size - just give you an error if you don't use it. The autorouter (and "follow me" router maybe) will use it.

It is always worth looking through the user ULPs for any features that don't exist - someone may have written something.

Keith.