Hello.
I'd like to maximize the performance of my CC2430 design and therefore would like to follow exactly TI's design.
I already followed TI's reference design, related to components selection and schematic.
Now, I want to follow their PCB manufacturing, and therefore have a number of questions:
1. How many layers should the PCB have?
2. What should be the PCB's width (if it depends on the amount of layers - 2 or 4 - please specify the width for each).(in the 'CC2430+CC2591 according to swra214' I saw that you recommend 1.6mm 4-layer PCB, but i read here that you recommend 1.2mm 2-layer PCB, so i'm confused).
3. How many oz. of copper should the PCB use?
If it helps to answer the question, i'm using a single ended antenna.
Thank you very much for any help.
The CC2430Em reference design is at http://focus.ti.com/general/docs/lit/getliterature.tsp?literatureNumber=swrr012c&fileType=zip
. It has all of the information you are looking for. The following was taken for one of the read-me files.PCB DESCRIPTION:2 LAYER PCB 1.0 MM Dimensions in mil (0.001 inch) DOUBLE SIDE SOLDER MASK, DOUBLE SIDE SILKSCREEN, 8 MIL MIN TRACE WIDTH AND 8 MIL MIN ISOLATION.
Hi Stewart,
CC2591EMK reference design read-me file writes: PCB DESCRIPTION:4 LAYER PCB 1.6 MM Copper 1 35 um Dielectric 1-2 0.35 mm (e.g. 2x Prepreg 7628 AT05 47% Resin) Copper 2 18 um Dielectric 2-3 0.76 mm (4 x 7628M 43% Resin) Copper 3 18 um Dielectric 3-4 0.35 mm (e.g. 2x Prepreg 7628 AT05 47% Resin) Copper 4 35 um DE104iML or equivalent substrate (Resin contents around 45%, which gives Er=4.42@2.4GHz, TanD=0.016) 1. Does that mean that board is designed without a core, but only based on prepreg? 2. Which dielectric/isolator is finally used: Prepreg 7628 AT05 47% Resin or DE104iML? 3. What can one expect when used dielectric/isolator is replaced to: a. FR4 b. Rogers RO4350
CC2591EMK reference design read-me file writes:
PCB DESCRIPTION:4 LAYER PCB 1.6 MM
Copper 1 35 um
Dielectric 1-2 0.35 mm (e.g. 2x Prepreg 7628 AT05 47% Resin)
Copper 2 18 um
Dielectric 2-3 0.76 mm (4 x 7628M 43% Resin)
Copper 3 18 um
Dielectric 3-4 0.35 mm (e.g. 2x Prepreg 7628 AT05 47% Resin)
Copper 4 35 um
DE104iML or equivalent substrate (Resin contents around 45%, which gives Er=4.42@2.4GHz, TanD=0.016)
1. Does that mean that board is designed without a core, but only based on prepreg?
2. Which dielectric/isolator is finally used: Prepreg 7628 AT05 47% Resin or DE104iML?
3. What can one expect when used dielectric/isolator is replaced to:
a. FR4
b. Rogers RO4350
Hello
The "core" is between layer 2 / 3, it is the same basic material as the pre-preg but purchased as sheet stock to have a solid material to build the layers up on. They are both similar to FR-4.
If you were designing a narrow notch filter or resonant element for an oscillator with transmission lines the Er of the material would be very critical, but you are not. The majority of the matching is done in lumped elements (Ls and Cs) which may benefit from the lower stray shunt capacitance resulting from a thicker substrate or the Rogers material with a lower Er (3.66). A wave length in air at 2.4GHz is 12.5 cm, for microstrip it is scaled by 1/(sqrt Er) which is 6 cm for a Er of 4.3. A 0.5cm transmission line is only 8% of a wavelength at 2.4GHz and 3% at 1GHz. Whether the line is 50 or 65 ohms you will see little difference in the performance.
The impedance of a transmission line is set by its Width over the dielectric thickness (Height). That is from the top trace to the ground plane which is layer 2 on a 4 layer design. Note it does not matter how many additional layers there are or the total thickness of the board.When using a reference design it is important to maintain the W/H of the transmission line. If the W/H is 1.9 (for 50 ohms on FR4) on a 4 layer design with a .35mm layer 1 to 2 thickness and you switch to a single layer board that is 1.5mm thick the transmission line must get 1.5/.35 or 4.2 times wider. This is to maintain the W/H ratio and the designed impedance. Above I wrote the line impedance is fairly insensitive to small changes (+/- 15%) in width or the Er of the material. A change of 4.2 times is not little and would impact performance in a bad way.
At ½ ounce copper and up there is little impact of performance. As the material gets thicker the impedance will shift down very slightly. If you go thinner than ½ ounce copper its “skin depth” at 2.4GHz will exceed its thickness and will start to become lossy.
The Rogers material is very similar to FR4 but with a slightly lower Er (3.66) and a little less loss. A W/H of 1.9 is 50 ohms on FR4 and is 53 ohms on 4350 due to this difference. With one T line of less than 10% of a wavelength you will never see the difference.
Stewart,
Thank you for the clear answer, very helpful.
Cheers,
Glasbergen
Hi Glasbergen, I've had some successes with CC2430 PCBS. Let me offer a little experience.
Impedance control is essential for good yield but don't try to second guess your PCB supplier on the properties of materials. You can take a first pass at the layout and call out nominal dimensions as a stating point. In the end your PCB house will know more about dialing in their process to hit a specific impedance. Call out a specific impedance for your RF traces on the fab drawing like “20 mill trace with a 10 mill dielectric over the RF ground plane equals 50 Ohms +/- 10% at 2.4 GHz” and let the guys at the fab house do the fine tuning. Most fab houses are doing high-speed digital PCB these days and impedance testing with Time Domain Reflectometers is common. Ask for a test coupon and report on your array.
The CC2430 reference design was, to put it nicely, and odd choice of dimensions: 40 mill dielectric thickness and 80 mill RF trace are uncommon, but that is what the stack-up works out to for 2.4 GHz. The PCB Balun is a conundrum. I would go with the Anaren Balun and take a look at the CC2511 PCB for a more rational approach to 2.4 GHz layout. Any more questions send me an e-mail.
RF
It is my first time drawing a PCB board and I am completely lost. I downloaded the CC2430EM reference design. But I do not know how it can be useful. I use Altium Design 6.6. The CadStar_files.zip in the folder includes a .pcb file but there is no way to import it to altium designer.
Right now, I only understand PDF files in CC2430EM_PDF_RD.zip but they can not be imported to Altium Designer. I just got out of coding with CC2430 and started hardware design.
Can you please explain the meaning and usefulness of files in these folders, like which are for reference only, which can be imported to Altium Designer? The folder TI provides should be of industry standard but I did not read any articles explaining how to start with such standard PCB information.
Besides, I am not sure how to draw a transmission line in altium designer. How is transmission line different from a normal PCB line?
Thank you very much.
Hello Arbi,
This is Chris Pinter with Pinter Electronics Consulting. I am an RF Engineer and while offer you some suggestions. If you need to get a hold of me directly please visit www.pinterec.ca
To answer your questions:
1. Generally speaking a RF board can have as many layers as you need. However the layer right under the components needs to be flooded with ground to eliminate noise and channel return current. The TI evaluation boards are all two layer boards where the bottom board is flooded with a ground layer. Note there are also many via holes to ground.
2. The PCB width can be any width you like. However the transmission line width will need to be adjusted for impedance and routing depending on the width, or distance between layers. The width of 1.6 mm 4 layer and 1.2 mm 2 layer is giving you two different options. The key point to note here is the transmission line width is not defined. That is the important missing information.
3. The amount of copper you should use depends on the current that will go through the trace and the PCB fabrication process. Generally speaking for RF designs I use 0.5 oz or 1 oz.
Doing a layout for an RF circuit can be very complicated and if you need more help just give me a call.
Hope this helps,
Chris Pinter
Senior RF Engineering consultant
I can try to help but there a lot of different subjects and disciplines involved assuming you are designing a custom board and not just trying to make more CC2430EMs. We will need to work together to get this done.
Altium Summer2009 has a tool to convert CADStar files, I have attached the converted files. They open in Altium 2009 and look good. See if you can open them in 6.6. The CAD Star library files were not available for conversion.
When I started designing my first board (I’ve now done over 50 boards) I spent a lot of time in the fog of which tool, can I find library parts, which fab house etc. I have since learned that is just not that hard. I suggest you capture the schematic in Altium first, get that right, I can go over it, and then worry about the PCB layout. PWB layout tools have a lot of features to make sure the layout matches the schematic provided they are linked.
The numerous files provided by Ti can be used in a number of useful ways. I’ve seen one person actually make photo masks using the pdf images and use them to etch the circuits. For the most part they provide a “reference” design. That is a design you refer to as you do your new design. Since most designs are unique, sometimes fitting in key Fobs, and other shapes, some have features like Li-Ion battery charges, CODECs, displays, buttons, etc. The RF portion of the reference designs are more critical and must be replicated as close as possible.
Transmission lines in Altium are just another trace on the PWB. What makes them a transmission line is they have a specific electrical length and impedance over a specific frequency band. Length is pretty clear; impedance is dependent on the width (w for width) of the line, the thickness (h for height) of the board material between the line and the first ground plane, and the dielectric properties (Er) of the board material. Sharp bends and other material placed too close to the line will affect its impedance. To a lesser extent the thickness of the line affects impedance. Assuming ½ to 1 oz copper the lines are thin enough that this effect is secondary.
Impedance – A perfect line can be modeled as L’s and C’s. While it is expressed in ohms it is not a resistance. A line that is roughly twice (w/h = 1.95) as wide as the dielectric is thick (e.g. 20 mils wide / 10 mils board thickness) on standard FR4 PWB material will have an impedance of close to 50 ohms. If a length of such a line is connected to a 50 Ohm resistor and a wave sent down the line, all of the waves energy will be dissipated in the resistor and very little of it will be reflected back towards the signal generator. Thus the line is said to have a characteristic impedance of 50 ohms. This is rather long but the take away is if the number of layers or other factors change the board thickness between the transmission line and the first ground plane the width of the line will have to change to maintain the line impedance.
After reading cc2430 datasheet, I understand it a bit more. I downloaded a trial verison Altium Designer 09 Summer. It works. Now I know basics about antenna and balun.
Hi Stewart. I would like to ask a few more questions since you also use Altium 2009. I am using Altium Designer 2009 Summer. I converted both CC2430DB reference design and CC2430EM reference design to AD 2009 Summer. CC2430EM looks fine and makes sense but CC2430DB looks very messy. I attach screenshots of them here:
CC2430DB:
:
CC2430EM:
CC2430DB's PCB layout is messy as you can see above, but the schematics still make sense. So I use CC2430DB schematics as a reference for my customized design. After 1 day's of work, compilation is successful. However, the components converted from Cadstar do not correspond to any package in AD 2009 Summer (after I ran "Import Changes From xxxx.PrjPCB", in "Engineering change order", I got a lot of RED cross marks with error message like "unknown pin: Pin xxx,xxx" which suggests components do not correspond to packages ). Did you replace those resistors, capacitors by components that can be found in AD 2009 manually?
Also, I am not sure even if I can successfully convert schematics to a PCB, it will be different from the PCB layout provided in the reference design. So what I have to next is to tidy the PCB so that it looks almost identical to that in the reference design (at least in the antenna part)?
TI suggests that we'd better follow reference designs as close as possible. Does it mean that after we obtained PCB from schematics, we replace the antenna and balun parts by that in the reference PCB design?
Apologize for the long question. Thanks if you can take a look.
Hello,
I imported CC2430DB into AD Summer09 Sp1 and got the same results as you. I used Tools/Component placer to expand the parts into something where I could at least see all of them. Obviously something is getting lost in the translation and while this layout might be optimized for minimum net length it is certainly NOT a suitable layout. The schematics opened nicely but as outlined below they are just “art”.
If you would like I can “walk” you through the first PCB design. The first step is selecting the right tool. I think Altium is best out there but its $3995 (be sure they throw in a nanoboard) and a 30 day trial may be a bit short. One approach is request a longer period, like 6 months or more, or use a free download (I like pcb123). Altium is a serious tool and a good skill to have.
The Ti reference design files for CADStar do not include the library files thus the schematic files are basically just “art”. Step one is to go through and assign symbols from the AD library to the schematic and create the ones not available in the AD library and assign them to the symbols on the schematic. Now you can go through and assign footprints to the symbols on the schematic. Many are in the AD library, I can send you some and you will need to make a couple. They are easy with a little guidance. I see people hung up because a foot print or symbols is not available and I do not understand this. They are quick to make and every time I use one from a library I seem to have a problem with it.
Notice everything so far is the schematic. The schematic in PCB design is King. The PCB layout tool will not let you make a connection different from the schematic, it is the source of foot prints and pin allocations. Once the schematic is complete you are 90% done. All that would be left to do is set the layer stack up in Designs/Layer Stack Manager, assign the planes, print the layer_1- CC2430DB_1_3.pdf file and place the parts as shown and connect them.
Last the CC2430EM is a good starting place (you still need to complete the schematic with symbols and footprints). By adding a debug header, and a power connector you would have a complete unit and it would still be compatible with Ti Flash program, Packet Sniffer, and RF Studio which are all free down loads. You could add a header to access a few SPI and GPIO inputs, a couple of LEDs, a push button for further utility.
Let me know how you want to proceed. My guess you can nail the CC2430EM schematic is a couple of days and have the tools to take on the DB design mostly on your own.
I really appreciate your generous help. Your explanation clears most of my doubts and I made a lot of progress today after reading your reply. After spending a whole day drawing the schematics as you suggested. The compilation is successful. I was able to create the netlist and went on to convert the netlist to PCB. I did not start sorting the components in PCB yet.
And thanks for your kind offer to review my PCB. Hope you do not mind a few more questions.
1. You suggested drawing PCB according to " layer_1- CC2430DB_1_3.pdf". CC2430DB has 4 layers. Does it mean when I use PCB Board Wizard to initialize my PCB, I should select 2 power planes and 2 signal planes, and make the board parameters (like each layer's thickness, material used, etc) are exactly the same as CC2430DB? Can I choose 2 signal planes and 0 power planes (because I think 2 layer is cheaper and maybe later easier to debug)?
2. If I use 2 layers, that means I can not copy and paste from the reference design since substrate thickness affects microstrip's characteristic impedance. Am i right?
3. In CC2430 schematics, there is a brown-out circuit in Power Source sub-schematic. CC2430 SOC has a built-in brownout circuit. So the brown-out circuit isn't necessary, is it?
4. I am not sure if this is right. For crystal, capacitor values, I just put the value in Designator entry in Component Properties. The PCB fab house will know which component to put by looking at my schematics, right?
5. Suppose I finished the PCB, I just send the PCB related files to the fab house. I requested a few free samples of CC2430 SOC chips. Should I give them to the fab house and tell them to solder on the right places? Can I also assume the fab house has crystals, capacitors, headers, pushbuttons, etc?
Next, I will sort out the components in the PCB generated and copy the antenna and the balun parts to my PCB. I'll send it to you after completion.
1.) 2 versus 4 Layers Your first consideration was cost. Using pcb123 V2 which gives instant quotes as you enter configurations a 1.5" X 1.5" board was $252 for qty 10 2 layer boards and $289 for qty 10 4 layer boards. $38 bucks or <$4 per board. The biggest saving, over $150, is to not have a solder mask, but given 0402 size parts and QFN packages this is not practical. Once you have a solder mask having the designators silk screened onto the board is free. The advantage of 4 layers with power and ground planes is anywhere you need either power or ground you pop in a via and you are connected. Thru hole part and connectors VCC and GND pins are automatically connected These planes are continues sheets on copper with only a small clearance around other vias. With ground on layer 2 you are guaranteed a continuous ground plane under everything on layer 1.
The disadvantage of 2 layers is power is one more trace that must be routed point to point and you will find it goes everywhere. Having all of these extra traces does not help trouble shooting. It is mandatory you have a continuous ground without breaks from the start to the finish under of all RF lines. On simple boards using a copper pour connected to ground on both sides of the board this can be done. A quick look at the C2430EM is a good example. As complexity increases it approaches impossible fairly quickly.
2.) Due to the need to route power and ground from pin to pin there is a lot of effort to port a 4 layer design onto 2 layers while maintaining a good continuous ground plane under the RF lines. It is not a simple cut and paste. Yes, the ratio of the width of the line (w) to the height ((h) thickness) of the board must be maintained for a given board material to maintain a certain impedance. The total thickness of the board does not matter, just h from the signal line to the ground directly under it.
3.) I’ll have to look at the brown out circuitry tomorrow.
4.) Designators are things like C4, R2, U1. In Altium if you click a schematic symbol and it shows green dots you can right click it and select properties. Here you can change the designator, enter the value (eg 10K, 1uF, 27pF), Red) and many other things such as supplier data as well as assign a footprint. The value entered here shows on the schematic and parts list and can be used by the assembly house. If you click on the designator and get gray squares and select properties you will see “Designator -- Value”. It wants the “value” of the designator, like R2, it does not want 10K, this caught me the first time also.
5. This is the question with the longest answer. Here is a short version that leaves out a lot. This is for a small run of 2 to 10 boards. Large jobs (1000 boards) have far more options.a.) You well need to have a parts list that includes the manufactures part number for each part you use. You can add this info into Altium and it will print the list. I use Excel and can send an example. The Ti part list for the CC2430EM is a fair example.b.) Most often you order the board from a PCB fab shop and supply it to the assembly shop just like other parts. A few PCB fab shops are starting to offer small run assembly services.c.) Small run assembly houses are all different. They differ on how they want the parts supplied. Some will accept loose parts, some charge to tape your loose parts – other don’t, others will take short pieces of taped parts and others want full reels. Many will take a combination. That is they will accept your unique parts in loose (generally called bulk) packaging and will supply common parts such as bypass caps and resistors. Since they buy these common parts on full reels (up to 10,000 caps on a reel!) they get good prices and using reels they can use automatic pick and place machines. You need to design to their available parts inventory.d.) Many of the companies I work with on this forum have an assembler or two and build their own boards.
It would be interesting to hear what shop other have found and how it is working for them.
Personally I build all of my prototype boards using the following approach:a.) Order the PCB from a fab shop. Order the parts from digikey.com, mouser.com and others.b.) Order the solder stencil ($125) using the Altium Gerber file for the paste layer.c.) Apply solder paste to the board using the stencil using a squeegee, using a microscope and a vacuum pick stick the parts in the solder paste. I then put it in a toaster oven until it reflows, the solder pulls all the parts into the right place, interesting to watch. Then I finish by hand soldering the thru hole parts. Then test. Figure 30 minutes for a board. By the time you are set up to trouble shoot and rework a board to get it to work the first time you’re probably set to assembly it as well.
After a few boards and the bugs are worked out I use a full service assembly shop supplying the unique parts on reels while using their common part also from reels. First run we’ll buy 100 to 500 boards.
Your reply helped me a lot in drawing my PCB. Thank you a lot. Now, I have my PCB drawing ready. I put it in my files area in this forum or you can access it from here (http://e2e.ti.com/members/1186100/files/CC2430PCB.zip.aspx). It is based on CC2430DB and simpler than it. I deleted EEPROM, joystick, temperature sensors, etc and I replaced the original accelerometer by a more advanced accelerometer ADXL345 from Analog Devices. I used Altium Designer Summer Build 9.0.0.17654.
Hope you don't mind a few more questions again.
1) Regarding your answer for my question (4) , can the designators be any value? I mean R3 and R303 do not matter, but their corresponding values are important, right?
2) Is manufacturer part list the same as BOM? In my BOM, the capacitors are grouped together under one row, which is different from the BOM for CC2430 which grouped capacitors by their values.
3) Under the antenna of CC2430DB, there is no GND and VDD. I am not sure how to get rid of this area of power planes so what i did is placing the antenna out of the board area. Is is right?
4) Should the polygon pour connected to GND or VDD or left unconnected?
I am very much appreciated that you take the time to have a look at my PCB. :-)
Hello I'll open the pcb file later this morning. First the questions:
1.) Designators: Once again everything comes back to the schematic where the foot print and designator are associated with a symbol. When you go to layout the foot print and designator go together. Designators are just labels and can be any number letter combination. You can use R1 but Rtherm, CAT or COW303 works to.
2.) Here are a couple of lines from my parts list:
You can see the manufactures part number, the supplier part number, designator, qty etc. It is a PBOM, Priced Bill of Materials. If you are not looking at the manufactures data sheet for the specific parts you plan to order and use, it is nearly certain what you will end up with parts that do not fit on the PCB or a PCB layout for a part no longer available in the package / footprint you grabbed out of a library.
3.) You can not place parts out of the board area. PCB are made many on a sheet (called a panel) of FR-4 or similar. After they are fabricated the sheet is cut into individual circuit boards. The "board area" determines where the panel is cut. What you want to do is delete the Plane1 (layer 2 which should be ground) in Stack up Manager and replace it with a Layer in Stack up Manager. Much like you draw the Polygon Pour on the top and bottom of the board you can add the Polygon Pour to this new layer. The important part is since you draw it you can decide what areas to leave un-filled. A Plane is the same thing and it is nice because it automatically covers the whole area but is not the way to go when you want multiple planes or in your case an area without a plane.
4.) The Polygon pour is typically connected to ground (GND) on the Top, Bottom, and Layer 2.