Post by thread:[EE] Eagle ERC questions

Hi, Been a while since I posted. Anyway, I am designing a board in Eagle, and when I do an ERC check on the schematic I get this error. SUPPLY pin GND overwritten with more than one signal(H-GND, GND) I changed the net class for those pins to be H-GND for a heavier trace width. I am not sure where it's getting the GND signal from ? I tried the archives and google, etc... but no luck. I basically have the GND pins on the M33887 chip tied to a GND symbol and then changed the net class to H-GND so that it has the track width set at 60 mils with 15 mils of clearence. Thanks, Kevin

Hi Kevin, I'm relabeling this [EE] since it fits better there and you'll get a wider audience. Kevin wrote: {Quote hidden}> Hi, > > Been a while since I posted. Anyway, I am designing a board > in Eagle, and when I do an ERC check on the schematic I get > this error. > > SUPPLY pin GND overwritten with more than one signal(H-GND, > GND) > > I changed the net class for those pins to be H-GND for a > heavier trace width. I am not sure where it's getting the > GND signal from ? > > I tried the archives and google, etc... but no luck. I basically > have the GND pins on the M33887 > chip tied to a GND symbol and then changed the net class to > H-GND so that it has the track width set at 60 mils with 15 > mils of clearence. > > Thanks, > Kevin

Thanks Bob. I basically have five net classes in Eagle v5.1 signal,gnd20,gnd40,pwr20, and pwr40. The gnd20 goes to the logic chips, and the gnd40 goes to the motor control chip. If I use the INFO command I can change NET CLASS, but not the NET NAME. It says to use the NAME command to change the name. If I use the NAME command it won't let me use the NET NAME I want it says already in use and tries to connect the NET class with the old name. I just wanted to run heavier tracks (40mil) for the 12V motor chip and 20 mil for the logic chips. Can I do this in Eagle ? I tried an old v4.15 but, it says I need at least v4.60 to open the schematic. Thanks, Kevin {Quote hidden}> Hi Kevin, > > I'm relabeling this [EE] since it fits better there and you'll get a > wider audience. > > Kevin wrote: >> Hi, >> >> Been a while since I posted. Anyway, I am designing a board >> in Eagle, and when I do an ERC check on the schematic I get >> this error. >> >> SUPPLY pin GND overwritten with more than one signal(H-GND, >> GND) >> >> I changed the net class for those pins to be H-GND for a >> heavier trace width. I am not sure where it's getting the >> GND signal from ? >> >> I tried the archives and google, etc... but no luck. I basically >> have the GND pins on the M33887 >> chip tied to a GND symbol and then changed the net class to >> H-GND so that it has the track width set at 60 mils with 15 >> mils of clearence. >> >> Thanks, >> Kevin > -

On Jul 20, 2008, at 6:59 PM, spam_OUTkbenTakeThisOuTdca.net wrote: > Can I do this in Eagle ? I tried an old v4.15 but, it says I need at > least v4.60 to open the schematic. The short answer is "no." It is a FAQ and an often-requested feature to allow one signal name to have multiple classes (especially analog vs digital gnd, and Power vs the short traces to fine-pitch SMT pins), but the "one class per signal" bit seems to be very entrenched in the design, so it hasn't changed in a long time and doesn't look like it's likely that it WILL change in the foreseeable future. The usual fixes involve various sorts of zero-ohm resistors used to connect the nets with the same potential but different names, or separate routing steps before and after changing the class definition, or manual routing, or living with lots of design rule warnings (one thing that IS possible in v5.x is to tell eagle to ignore certain warnings.) BillW

On Mon, Jul 21, 2008 at 1:07 PM, William Chops Westfield <.....westfwKILLspam@spam@mac.com> wrote: > > On Jul 20, 2008, at 6:59 PM, kbenKILLspamdca.net wrote: > >> Can I do this in Eagle ? I tried an old v4.15 but, it says I need at >> least v4.60 to open the schematic. > > The short answer is "no." It is a FAQ and an often-requested feature > to allow one signal name to have multiple classes (especially analog > vs digital gnd, and Power vs the short traces to fine-pitch SMT > pins), but the "one class per signal" bit seems to be very entrenched > in the design, so it hasn't changed in a long time and doesn't look > like it's likely that it WILL change in the foreseeable future. Hmm, do you know any EDA package to allow one net name to have multiple Net Class associations? As far as I know, Altium P-CAD does not allow that. Mentor Graphics Expedition Design Capature does not allow that either. > The usual fixes involve various sorts of zero-ohm resistors used to > connect the nets with the same potential but different names, or > separate routing steps before and after changing the class > definition, Last time we tried this with P-CAD and it did not work too well. > or manual routing, I believe this is the way to go. >or living with lots of design rule > warnings (one thing that IS possible in v5.x is to tell eagle to > ignore certain warnings.) We still use the design rules to check the creepage/clearance between different Net Class. However, manual check is also necessary. Sometimes we need to get the help from Mechanical Engineers (inside Pro-Engineer) to check 3-D distance. Xiaofan

I'll look for the FAQ, I read the tutorials and did not see an answer to my questions. But, maybe I am dense I don't want one signal with multiple classes. I have two classes and two signal names. I.E. I want all A-GND signals to use the GND40 (40mil) class and all D-GND signals to uses the GND20 (20mil) class. Surely this is possible ? Regards, Kevin {Quote hidden}> > On Jul 20, 2008, at 6:59 PM, .....kbenKILLspam.....dca.net wrote: > >> Can I do this in Eagle ? I tried an old v4.15 but, it says I need at >> least v4.60 to open the schematic. > > The short answer is "no." It is a FAQ and an often-requested feature > to allow one signal name to have multiple classes (especially analog > vs digital gnd, and Power vs the short traces to fine-pitch SMT > pins), but the "one class per signal" bit seems to be very entrenched > in the design, so it hasn't changed in a long time and doesn't look > like it's likely that it WILL change in the foreseeable future. > > The usual fixes involve various sorts of zero-ohm resistors used to > connect the nets with the same potential but different names, or > separate routing steps before and after changing the class > definition, or manual routing, or living with lots of design rule > warnings (one thing that IS possible in v5.x is to tell eagle to > ignore certain warnings.) > > BillW > > -- Kevin

> SUPPLY pin GND overwritten with more than one signal(H-GND, > GND) Eagle thinks the name of the net connected to a supply pin should be the same as the name of the supply pin. I think that's a silly rule and makes the ERC less useful, but there is no way to shut it off that I know of. You just have to go thru all ERC warnings and make sure none of them are "real". ******************************************************************** Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products (978) 742-9014. Gold level PIC consultants since 2000.

kben@dca.net wrote: > I basically have five net classes in Eagle v5.1 > signal,gnd20,gnd40,pwr20, and pwr40. > The gnd20 goes to the logic chips, and the gnd40 goes to the > motor control chip. You are confusing net classes with the net name. Each net can only have one class and one name. You can't assign one class to a part of a net and another to the rest. I usually use one of two solutions. The first is to manually route critical parts of nets. You probably want to do this anyway if you need large current capability since you don't want those tracks going all over the place and you want to keep the current loops to a minimum and you have to carefully think about ground offset voltages. You can manually route with any width and drill size regardless of the net class. I usually manually route all ground connections because I usually have a ground plane or pseudo ground plane. In those cases, I want each ground SMD pad with its own via straight to the ground plane. This is usually better for the signals and makes subsequent routing easier. The second method is to break up a logical net into multiple Eagle nets by using "short" devices. These are just copper with two connections. I draw them as a slightly thickened line on shematics. To Eagle each side of the short will be a different net. This technique is particularly useful to guarantee that the ground connection for some part of the circuit connects at exactly one point that you can place to the rest of the circuit. This allows you, for example, to keep switching power supply loop currents isolated and off the main ground plane. ******************************************************************** Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products (978) 742-9014. Gold level PIC consultants since 2000.

No, I have two nets, and two classes, with different signal names. It must be a bug in v5.1, or a prodedural error. I was able to delete all my Digital Grounds and then change the net and class to what I wanted. Analog GND, Net Name "A-GND", Net Class "GND40" Digital GND, Net Name "D-GND", Net Class "GND20" Regards, Kevin > Kevin wrote: >> I have two classes and two signal names. > > But I thought you were trying to apply them to one net. Each net can have > only one name and one class. >