Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Draw component with cadstar
- Thread starter pucca
- Start date
Have you looked to see if a library for the part already exists? Typically both component manufacturers and the tool company both supply libraries. This would greatly simplify the work.
Otherwise you will be in for a bit of work. I haven't used Cadstar, but I imagine the process is similar in all tool sets. First you will need to create a symbol definition that will represent the component on the schematic. Then you will need to create the PCB land pattern that will define the component on the PCB. The tool will provide some means to correlate the symbol pins to the PCB pattern pins. If you go through the documentation and the tutorials you will likely find several examples of how to do this.
Given the 'how to' you will need to reference the data sheets VERY CAREFULLY and ensure that your pad definitions and spacings will fit the part, while still maintaining sufficient clearances, etc.
Honestly I am not sure starting with the microcontroller fo r your first part is a wise move. Instead start with some chip components then move on to some SOIC devices, and after you are comfortable then try the microcontroller. In the end, you might be able to get a decent quality plot or print from the design files and with this you may be able to determine if the part will fit by placing a real one on the paper.
Otherwise you will be in for a bit of work. I haven't used Cadstar, but I imagine the process is similar in all tool sets. First you will need to create a symbol definition that will represent the component on the schematic. Then you will need to create the PCB land pattern that will define the component on the PCB. The tool will provide some means to correlate the symbol pins to the PCB pattern pins. If you go through the documentation and the tutorials you will likely find several examples of how to do this.
Given the 'how to' you will need to reference the data sheets VERY CAREFULLY and ensure that your pad definitions and spacings will fit the part, while still maintaining sufficient clearances, etc.
Honestly I am not sure starting with the microcontroller fo r your first part is a wise move. Instead start with some chip components then move on to some SOIC devices, and after you are comfortable then try the microcontroller. In the end, you might be able to get a decent quality plot or print from the design files and with this you may be able to determine if the part will fit by placing a real one on the paper.
- Thread starter
- #3
Where can I download atmel library files? I found some at
but they are .lbr files and cadstar uses .lib
but they are .lbr files and cadstar uses .lib
- Thread starter
- #5
- Thread starter
- #7
Honestly, that may be the easier approach. I think in all the PCBs I did, I used a pre-done libarary for a part once.
I am willing to bet that you have already spent more time searching for an off the shelf solution than it would have taken to create the part yourself.
The process ins't too difficult, nor would I say it is risky. You will need to use the data sheet and or packaging info sheet to get the paramaters. The tool I am most familiar with is PCAD so I will give you an example from that.
You will first create the schematic symbol by specifying a rectangle of X by Y inches and the number of pins you want on each of the 4 sides. This isn't critical, its a matter of preference. You then specify, starting at pin 1, what you want to name the pin and procede to do this with all the pins. You then create a PCB pattern, which again will be based on a rectangle of U by V inches or milimeters (consult datahseet). I said U by V to emphasise that this is not the same dimension as used in the schematic. I ususally use the IC body definition for this and add a little bit, say 0.01". The datasheet will give you a pin length, width and pitch. You then define pad styles, which I make about .02" to .05" longer than the length, and usually equal to the pitch. you then specifiy the pin-pin spacing in the tool (this is the pitch) and the number of pads per side. This places the pads, spaced according to the part pitch with the rows centered (seperated) by the IC body dimension. I then measure and compare versus the datasheet to make sure that my pads cover slightly more than the worst case dimensions of the device and that I have (at least) about .007" between the pads and that my pads are slightly wider than the pin width.
Finally, when I have the symbol and the pattern, the symbol pins get tied to a corresponding PCB pin by way of the pin designator, which I almost always set to the pad number.
I have used this process several times with flat pack devices upto 244 pins. It hasn't failed me yet.
I am willing to bet that you have already spent more time searching for an off the shelf solution than it would have taken to create the part yourself.
The process ins't too difficult, nor would I say it is risky. You will need to use the data sheet and or packaging info sheet to get the paramaters. The tool I am most familiar with is PCAD so I will give you an example from that.
You will first create the schematic symbol by specifying a rectangle of X by Y inches and the number of pins you want on each of the 4 sides. This isn't critical, its a matter of preference. You then specify, starting at pin 1, what you want to name the pin and procede to do this with all the pins. You then create a PCB pattern, which again will be based on a rectangle of U by V inches or milimeters (consult datahseet). I said U by V to emphasise that this is not the same dimension as used in the schematic. I ususally use the IC body definition for this and add a little bit, say 0.01". The datasheet will give you a pin length, width and pitch. You then define pad styles, which I make about .02" to .05" longer than the length, and usually equal to the pitch. you then specifiy the pin-pin spacing in the tool (this is the pitch) and the number of pads per side. This places the pads, spaced according to the part pitch with the rows centered (seperated) by the IC body dimension. I then measure and compare versus the datasheet to make sure that my pads cover slightly more than the worst case dimensions of the device and that I have (at least) about .007" between the pads and that my pads are slightly wider than the pin width.
Finally, when I have the symbol and the pattern, the symbol pins get tied to a corresponding PCB pin by way of the pin designator, which I almost always set to the pad number.
I have used this process several times with flat pack devices upto 244 pins. It hasn't failed me yet.
- Thread starter
- #9
I really can't speak for what a particular vendor has done in thier product that uses this part.
Go to Atmel's website and download the datasheet. On page 369 you will find packaging information. Assuming your using the 64A package, the device has a height and width of 16mm. Therefore you want your PCB land pattern (pads) to be about 16mm on center, measured across from the device. The pins have a max lenght of .75mm, so I would make the pad length a bit longer, call it 1.0mm to 1.2mm. Adjustment will be required once you see how it looks on the screen. The pitch is .8mm so I would make the pads .8mm wide to start (this is wider than the .45mm pads). Then see if you have enough clearance.
Once you have the rough dimensions, measure everything and make sure that a device with min and max tollerances fits on the pattern as drawn. Also make sure you have sufficient cleaning clearance (about .010") from where the pins form/bend to the package body and between the pins.
Don't look into this too deep. It is not an exact science. You want to make sure there is plenty of room for the pads, etc. As long as you have things properly covered and enough clearance, it will be fine. There is no one right answer.
Go to Atmel's website and download the datasheet. On page 369 you will find packaging information. Assuming your using the 64A package, the device has a height and width of 16mm. Therefore you want your PCB land pattern (pads) to be about 16mm on center, measured across from the device. The pins have a max lenght of .75mm, so I would make the pad length a bit longer, call it 1.0mm to 1.2mm. Adjustment will be required once you see how it looks on the screen. The pitch is .8mm so I would make the pads .8mm wide to start (this is wider than the .45mm pads). Then see if you have enough clearance.
Once you have the rough dimensions, measure everything and make sure that a device with min and max tollerances fits on the pattern as drawn. Also make sure you have sufficient cleaning clearance (about .010") from where the pins form/bend to the package body and between the pins.
Don't look into this too deep. It is not an exact science. You want to make sure there is plenty of room for the pads, etc. As long as you have things properly covered and enough clearance, it will be fine. There is no one right answer.
I can't speak for all s/w vendors, but found libraries ready to be added to projects, from Altium support center for earlier s/w versions, P2P programs, College/Univ. websites, and even some amateur electronics blogs.
Check the datasheet or the ATmel website for similar devices/replacement parts, for a wider search scope. ATmega128 is pin2pin compatible with the older and more popular ATmega103, so you may look for '103 libraries, change some pin names and you're done. Good luck.
Check the datasheet or the ATmel website for similar devices/replacement parts, for a wider search scope. ATmega128 is pin2pin compatible with the older and more popular ATmega103, so you may look for '103 libraries, change some pin names and you're done. Good luck.
- Status
Similar threads
- Locked
- Question
- Locked
- Question