----- Original Message ----- From: "Brian Guralnick" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Thursday, August 14, 2003 4:57 PM Subject: Re: [PEDA] PCB Copper thickness VS mounted rails.
> > The problem with calling out 4 oz. Cu, or even 2 oz. for that matter, is > > that the board house will probably "pattern plate" the Cu, and it may not > be > > uniform. There is additionally the problem of etching small traces in the > > same layer, due to the thickness. > > My PCB house says that their process is a positive growth of copper, not > an etch process. Is this your described "pattern plate"? When you say "not > uniform", how much error can I expect? Will it matter with traces from 50 > mil to 500 mil. > > My PCB does not have any fine traces. It's a pure CMOS class A audio amp > and power supply. 3-4 traces are 25 mil wide (audio in), everything else is > at least 50 mil wide, mostly 250 mil wide. > Most boards today have at least one "additive" process, where the outer layers and all of the drilled holes that are to be "plated thru", get a layer of electrically plated copper. This usually follows a non electrical plating process where there is a small amount of "electroless copper" (copper that is plated / deposited chemically) plates the entire board, including the inside of the drilled holes, so that the entire board (including the inside of the holes) can be electrically "charged" so that electrical plating process will extend into the holes. Typically, this electrical plating process may plate an equivalent plating thickness of from 1/2 ounce to 1 ounce of copper, or more. Thus if you specify 1 ounce of copper for the outer layers of the board, your board house may start with 1/2 ounce (or less) copper foil on top of several layers of prepreg, or use a laminate with 1/2 copper (depending on the stackup), and then "plate up" an additional 1/2 ounce of copper (after the electroless process), so that the final thickness of copper on the outer layers is a full 1 ounce, and the copper wall thickness inside the holes is approximately 1/2 ounce. This process can vary greatly, depending on just how much copper you specify on the outer layers and what you want in the wall thickness of the plated thru holes. Once the copper is plated up to the final thickness, the board is then usually masked with the trace pattern and then etched. There are a few variants to this process. First, there is the process whereby all of the copper that is to be placed on the board is added thru selectively plating copper only in the areas where there is to be copper in the final board. This is an additive process only, and involves no etching away of any unwanted copper. This process / method of making boards has been around almost as long (if not longer) as the etching process, and has been very popular "offshore" where very large quanties of boards are made and where this process can save lots of money by not only needing as much (or little) copper as you are actually going to use, but additionally in the saving of the cost of etchant and echant disposal. Another process, which combines the best of both worlds, is used quite often by many vendors today. This is the "pattern plating" process (although you could easily apply this name to the previous process, and this process may go by different names in some locals). In this process, you begin with a thin layer of copper on the outer layers (or any other layers for that matter), of say 1/4 or 1/2 ounce, and then you electrically plate up the remaining thickness of copper (with or without "electroless" plating as may be required for plated thru holes). The difference here, is that you first mask the thin starting layer of copper with an inverse image of the final copper traces and features, so that you will only plate copper in the areas that are to have copper in the final design. The next step in this process would then be to clean off the original mask and then remask only the areas that you have plated up (which masking can even be done by plating the conductor pattern with solder, if you use the proper etchant), and then you etch away the small amount of unwanted copper which remains from the starting layer of 1/4 or 1/2 ounce copper. Aside from the normal benefits of using less copper and extending the life of your etchant, there is another major benefit with this process in that it can yield much better control of very fine copper features (traces / lines / etc,) since there is much less copper to be etched (thickness wise), and much less "undercut" in the etching process. Thus the primary advantage of this process, is the control of finely etched features. However, there is also a major drawback in using this process, in that when the entire thin starting layer is masked, and then when the board is electrically connected to the plating supply (which makes the whole board become an electrode in the plating process) and immersed in the plating bath, the amount and distribution of the mask on the thin starting copper can affect the distribution of the charge of the surface of the electrode (which is now the board itself), which can cause different thickness of copper to be plated in different areas of the board. This type of uneven plating can be controlled to some extent by trying to distribute the amount of copper that is being used in the design evenly over the entire surface of the board. Sometimes your board house may add what are called "robbers" or "thieves" to accomplish this. Some people call this "balancing" the distribution of copper on a layer, but please note that this term can easily be confused "balanced copper" or "balancing the copper" in the design, which is the much older and much more common usage, which refers to "balancing the copper" placement in the board stackup to prevent board warpage and delamination. Back to the problem at hand. Your board shop will probably not start with 4 ounce copper, and then etch thru all 4 ounces. Most likely they will start with a much thinner starting layer, and then "pattern plate" up to 4 ounces, or they may even do everything by a totally additive process (I would think that they are using a normal "pattern plating" process with at least some etching involved, notwithstanding what they may have told you, and which you mentioned aboved). Whether simply plating a full 4 ounces, or pattern plating 2 or 3 or more ounces, I am sure that there are liable to be several areas on your board which will present a real challenge to totally even plating resulting in totally even thicknesses. The thickness being the operative word here in identifying the problem. The small and minor differences in thickness encountered in normal pattern plating are going to be magnified several times in the thickness that you will be using (4 ounces). I would additionally be concerned with "overhang" in your process, which would be the opposite of "undercut" in an etching process, but which will surely be present to some extent in the plating (or "copper growth" as your board house appears to call it) thicknesses that you are dealing with. Will it affect your design. The answer is yes, no, and maybe, and it is all dependant on your board house. The real question is, can they guarantee a minimum thickness of 4 ounces of copper throughout your entire design, assuming that you want to use 4 ounces as the number in your current calculations. What is the difference in current carrying capacity for a given width of trace with a difference in thickness between 3 1/2 ounces of copper and 4 ounces of copper? Are we actually talking about this much difference in the thickness of copper? It all depends on how good your board house really is, but I would not rule it out if they are not paying real close attention, once again, due to the thickness. Remember that 1/2 ounce is 12.5% of 4 ounces, and most board houses only work to +/- 10 % on such things as thickness and stackup spacings. Now let me throw in one other variable here, to mess with everybody's mind. For years I have tried to find out what the difference is in molecular density between rolled copper sheet (which is very highly compressed due to the rolling process), and electroplated / electrodeposited copper (which does not undergo any compression, and which can very due to variables in the processes involved), such as that which we are talking about in the manufacture of a pc board. I have talked to many board houses and also many Chemists about this difference, and they all agree that most likely a there is in fact a real difference, but no one has been able to point me to a place to find out just what the difference really is, however, all agree that a difference in molecular density most probably would directly affect the current carrying capacity of the specific copper, especially where the amount of such copper was defined or controlled by its thickness. In other words, a copper trace, made from 4 ounce rolled sheet, will have a higher molecular density and therefore carry more current than a trace that consists entirely or mostly of copper that has been plated up to the same thickness as the 4 ounce rolled sheet. This actually is an interesting problem, and I wish that I could find someone who had some real answers to this issue. The problem in this scenario is that all of the copper used in the manufacture of printed circuit boards today is defined by thickness, and only by thickness, notwithstanding the fact that those thickness were originally derived from the weight of a specific amount of copper rolled to cover a certain area, and the simple fact is that no one in this industry ever weighs copper, but simply measures its thickness. When dealing with only the thicknesses of the copper, the molecular density of the copper really does make a difference. Bottom line in your case, if you really are going to use 4 ounce copper, I would start with rolled copper sheet, especially since you say that there are no small features that would be affected by the under cut, and design the widths to account for the large undercut, or at a minimum, start with 2 ounce and plate up the other 2 ounces. Actually, as mentioned before (in my last post), I would split the trace into 2 layers (top and bottom) of 2 ounces each, with a liberal sprinkling of vias to stitch the 2 traces together. There is yet one other area where I would think that you might find a problem in your design, and that is one you have already mentioned in your previous post, and that is the area of a connection of such parts as a capacitor. While I asked in my previous post whether or not your capacitor was large enough to be available with a "screw mount", so that you could use both sides of the board as a point of connection, I would additionally think that it might be helpful in your design to think about soldering a lead on both sides of the board, if and where you can. While I would still opt for duplicating the high current traces on both sides of the board, especially in the area of "mounting pads", with numerous "stitching vias" between them, this would be an excellent manner of current distribution if you could access and solder both sides of your connection to the traces on both sides of the board. (even if you cannot access a joint on the one side of the board, if you use rosin and the right temperature iron and proper soldering technique (which I am sure you possess) you can still insure that the solder 'flows" thru the joint to the back side of the board). Once again I would point out that you would do well to use a much larger trace than any "current calculator" might recommend, if possible, since you really don't want to add a "10 degree C rise in temperature" (or more) to your amplifier, which is where all of the calculators begin their calculations. Anyway, hopefully all of this helpful to you and possibly others who may read it. JaMi * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
