Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-04 Thread Joe McCauley
Thanks for all the replies guys. I realise I was not very detailed in my
post, preferring to pose the question in general terms. The actual circuit I
have is as follows. 1 L298 H-bridge driving a stepper motor. The driver is
controlled by an L297 stepper motor controller. This generates the phase
sequence  PWM for the driver. The 'Ground' end of the H-bridge is connected
to ground through a current sense resistor. The net connecting the H-bridge
to the current sense resistor is the 3mm wide one. The motor current passes
through this net and the sense resistor to ground, hence the need for a wide
trace. The purpose for the sense resistor is to give current feedback to the
PWM generator. Routing the wide traces back to the L297 for feedback is not
really an option. The sense input on the generator is an opamp input. I
don't know if it is bipolar or not. Given that only short distances (6cm
total for the line from sense resistor to the opamp input) are involved I
can use a thinner trace (0.35mm). There is no separate ground sense line.
This configuration has worked fine for me in the past.

When I route a board I usually setup the width constraint for each net,
autoroute the board and then manually cleanup. In this case the auto router
will route the net using the 3mm thickness throughout. If the part of the
net which did not have to be so wide could have its width defined seperatly,
then the autorouter would route differently and probably better. The virtual
short thing sounds interesting  I can see how it works. I'm less sure how
the from-to width rule works never having used it.

Thanks for all the feedback.

Joe





* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread John A. Ross [Design]
 -Original Message-
 From: Joe McCauley [mailto:[EMAIL PROTECTED] 
 Sent: Wednesday, September 03, 2003 12:10 PM
 To: Protel EDA Forum
 Subject: [PEDA] Joining 2 different nets keeping seperate identifiers?
 
 
 I need to have a current return line with 3mm thickness. This 
 line has a net identifier of 'Iret'. This line connects to a 
 current sense resistor. I need to take a line from this 
 resistor to an amplifier input. There is no need for this 
 amplifier input line to be 3mm thick, in fact from the point 
 of view of routing it would be better if it were not! Is 
 there a way of joining 2 different nets in the schematic 
 while keeping seperate identifiers? If there were then I 
 could setup the design rules in PCB to always have the 'Iret' 
 net 3mm thick, while the other one which connects to it could 
 be (say) 0.35mm. Am I over complicating things by trying to 
 do it this way?

Joe

Mr Lomax had a method to do this as a 'virtual short', a feature now
supported in DXP called 'net ties'. 

If you browse the archive you will find it.

But if this is a once only route, then you may find it less time
intensive just to do this route by hand.

Have you tried defining the 'from to' topology and applying a width rule
with filter set to from-to? Just an idea.

Best Regards

John A. Ross

RSD Communications ltd
Email  [EMAIL PROTECTED]
WWWhttp://www.rsd.tv
==  



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread JaMi Smith
Joe,

Who says it has to be a 3mm thickness (I think you may actually mean that
the trace has to be 3 mm wide)?

Is this requirement imposed on you by an Engineer, or is it some requirement
found in a datasheet for some specific circuit or device?

A current sense resistor has to be in series (in line like a fuse
would be) with the load (the circuit or voltage that is being sensed) so
that it can determine how much current is being used. In most cases a
current sense resistor is used so that there can be some feedback to the
circuit that is controlling the voltage output of some type of voltage
regulator (or voltage distribution), however, in few cases, it may be used
so that the current can be measured for some other reason such as to take a
measurement for a remote monitor of some kind.

In most, if not all cases, there needs to be a direct and unobstructed path
back to the feedback input of the controlling circuit (which in your case
is the amplifier input) which has no additional loss (such as a resistive
drop in the trace) which could otherwise affect the measurement. Typically,
this requirement may be met by  specifying a wide trace (such as your 3 mm
requirement) for the feedback signal, but more often, a very short and
direct trace can be used, which can  usually be accomplished by having a
good component placement so that the current sense resistor is not too far
away from the circuit involved (however, you must still watch out for any
direct feedback to the amplifier input from the other end of the current
sense resistor, which is usually the output of the controlling circuit
(in other words, the location of the sense resistor can be very critical)).

As stated above, the current sense resistor is in series with the load,
and this means that it is only there so that you can measure the current
going thru it (by forcing a very small and controlled amount of current
limiting), as opposed to being in the circuit for some other kind of
current limiting, which is the normal function of a resistor. This means
that the load side of the sense resistor (where you are also taking the
trace back to the amplifier input (for a feed back measurement)) is also in
most cases the supply voltage for whatever circuit is connected to this
load side of the current sense resistor. This would mean that it should be
a wider than normal trace so that it can handle the power distribution to
that circuit, just as if it were the normal VCC (or other power supply)
trace in your circuit if you were not using any internal planes for power or
ground distribution.

With that said, the real question that needs to be addressed here is just
how much current is going thru the sense resistor to the load.

It may just be that the 3 mm requirement in your case is for the load
itself, as opposed to the feedback line from the load.

On the other hand, if there is a very large load (on the output side of
the current sense resistor) that is being measured by the feedback
trace, then 3 mm might be a very appropriate width for the trace.

What is critical here, is that you do not want any loss or any other
variables in this feedback trace (which would affect the feedback
measurement) that may vary from board to board due to such things as
manufacturing processes (etching or plating differences or minute
differences it the copper (trace) thickness), or which may vary in the same
board from such things as the resistivity of the trace varying due to
changes in ambient temperature during operation.

All of this boils down to having a very good and direct path back to the
current sensing input of the amplifier in your application which will not
have any resistive loss or drop.

Thus the 3 mm width requirement.

In this case, I would additionally say that you do not want to have any
feedthrus or vias in this feedback trace, nor do you want to have anything
else in the trace that might in someway affect the resistivity of the trace.

A parallel response to this post, which deals with your wanting to use two
2 different nets (the subject of this thread), suggests that you might be
able to use two different nets as you request in your original post, and
then using the Lomax Virtual Short method to join your two 2 different
nets together. This would be a very good solution to your problem in just
about any other application but this one, since the Virtual Short plays
some tricks on Protel by having a very very small gap between the traces to
overcome DRC errors and objections, but which itself is reliant on the two
traces actually bridging or shorting the small gap (or more accurately,
not etching it thru completely, or bridging it with solder) during the
manufacturing of the board, which unquestionably will have a major impact on
the actual resistivity of the feedback trace involved. For this reason,
I would strongly advise you to not use the Lomax Virtual Short scheme, or
in any other way attempt to isolate the feedback trace from the load
side of 

Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread JaMi Smith
Joe,

Oops !!!

I actually forgot to the most important statement in my whole response,
although it is implied (I actually started to write it in one place, but
changed it and wrote something else, and then forgot to put it back in
another location).

The net name of the feedback trace, which in your case you said is Iret,
must (as in ABSOLUTELY MUST) have the identical (as in ABSOLUTELY IDENTICAL)
net name as anything and everything else connectet to the load side of the
current sense resistor.

It  IS   all the same net !!!

It ABSOLUTELY MUST be all the same net !!!

Your real problem is that you are trying to use 2 different net names !!!

If you, or your Engineer, or your datasheet, have a problem with this, than
do not put any name on that portion of the net on the schematic with a net
label at all, but put Iret in parenthesis (such as ( Iret )) in a text
string near the line on the schematic, or a text string that says NOTE:
Current Sense Return near the line.

Do anything but try to make it a different net !!!

JaMi

 - Original Message -
From: Joe McCauley [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, September 03, 2003 4:09 AM
Subject: [PEDA] Joining 2 different nets keeping seperate identifiers?


 I need to have a current return line with 3mm thickness. This line has a
net
 identifier of 'Iret'.
 This line connects to a current sense resistor. I need to take a line from
 this resistor to an amplifier input.
 There is no need for this amplifier input line to be 3mm thick, in fact
from
 the point of view of routing it would be better if it were not! Is there a
 way of joining 2 different nets in the schematic while keeping seperate
 identifiers? If there were then I could setup the design rules in PCB to
 always have the 'Iret' net 3mm thick, while the other one which connects
to
 it could be (say) 0.35mm. Am I over complicating things by trying to do it
 this way?

 Thanks for any pointers,

 Joe





* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread Ian Wilson
On 07:40 AM 4/09/2003, JaMi Smith said:
Joe,

Who says it has to be a 3mm thickness (I think you may actually mean that
the trace has to be 3 mm wide)?
Is this requirement imposed on you by an Engineer, or is it some requirement
found in a datasheet for some specific circuit or device?
I would expect that the spec is wide uncalibrated current carrying traces 
with narrow current *sense* traces running off to the sense 
amplifier.  This is a pretty standard sort of interface in high or 
precision voltage or current applications.  You take a pair of sense traces 
to the load or sense resistor rather than using the uncalibrated high 
current traces for both current carrying and sensing.  The 3mm width 
requirement would come from the expected current, while the thinner traces 
are used for the actual sensing. Very standard stuff.

(Many bench-top power supplies will have sense terminals that allow you to 
control the voltage at the load rather than at the supply terminals, there 
is usually weak feedback in the supply to ensure that the supply is 
controlled if the sense terminals are unconnected.)

The requirement is perfectly reasonable to me and I would either solve it 
by setting up from-tos and appropriate rules or by the Lomax Virtual 
short.  In DXP it could be solved by a net tie component.

Ian



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread JaMi Smith
Ian,

Please see below,

JaMi

- Original Message -
From: Ian Wilson [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, September 03, 2003 3:49 PM
Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers?


 On 07:40 AM 4/09/2003, JaMi Smith said:
 Joe,
 
 Who says it has to be a 3mm thickness (I think you may actually mean
that
 the trace has to be 3 mm wide)?
 
 Is this requirement imposed on you by an Engineer, or is it some
requirement
 found in a datasheet for some specific circuit or device?

 I would expect that the spec is wide uncalibrated current carrying traces
 with narrow current *sense* traces running off to the sense
 amplifier.  This is a pretty standard sort of interface in high or
 precision voltage or current applications.  You take a pair of sense
traces
 to the load or sense resistor rather than using the uncalibrated high
 current traces for both current carrying and sensing.  The 3mm width
 requirement would come from the expected current, while the thinner traces
 are used for the actual sensing. Very standard stuff.

 (Many bench-top power supplies will have sense terminals that allow you to
 control the voltage at the load rather than at the supply terminals, there
 is usually weak feedback in the supply to ensure that the supply is
 controlled if the sense terminals are unconnected.)

 The requirement is perfectly reasonable to me and I would either solve it
 by setting up from-tos and appropriate rules or by the Lomax Virtual
 short.  In DXP it could be solved by a net tie component.

 Ian


The initial question is not because I want or need to know why there is a
requirement for a 3 mm trace width, but so that Joe can understand what the
problem is, and just what the requirement may apply to.

While I wouldn't necessarily state what you did in your first paragraph the
way that you stated it, it does get the point across, and is not different
than mine (although stated somewhat backwards as compared to what I stated).
If you will carefully re-read my post, and also read the follow-up post with
what I forgot to put in the original, you will see that I am trying to
explain just where the high current is and where it goes, and just exactly
what the current sense resistor does, and what the requirements may be for a
feedback trace from the load side of that current sense resistor, and
what the 3 mm requirement may apply to.

If you will also carefully re-read the original post from Joe, you will see
that this requirement has nothing to do with remote sensing, such as in your
example in your second paragraph of the power supply, but that he is
directly taking a trace from the load side of the current sense resistor,
and feeding it directly back into the [current sense] amplifier input.

I am sorry for my omission in my original post, but hopefully with the
supplement from my follow-up post, it will all become clear.

Yes, my original post is a bit confusing, but I think that you will see that
we are saying the pretty much same thing, with respect to your first
paragraph above, and that your second paragraph really does not apply to
this instance.

Respecting your last paragraph, I am fairly sure that when you get my
follow-up post and think the whole thing thru together with the first post,
that you would concurr with me in what I stated in my follow-up post, that
the present case that Joe is describing, that the feedback trace is in
fact the same net as the net connected to the load side of the current
sense resistor (which in fact is just exactly what you yourself describe in
your first paragraph above), and that it really should not have a different
net name, and that the different net name is the real problem here (but
which would not be the case in the example of your second paragraph). That
said, I think that you would additionally concurr with my stating that
anything that would introduce any loss or drop in the feedback trace
should be avoided (such as the loss that would almost certainly be
introduced by unnecessarily using 2 differnt net names and trying to join it
all together with a Lomax Virtual Short (with its intentional gap which
can allow for some small and uncontrolled amount of etching of the trace at
the point of the gap), or by using too narrow a trace which could cause too
much restivity in the trace). I would also think that whatever DXP may or
may not do here does nothing but confuse the issue (especially if there is
no reason to have 2 different nets in the first place).

Sorry for any confusion, but I think you may be trying to say the same thing
as I did with respect to the present situation, and that the case for the
isolated remote sense (as you described in your second paragraph) does not
in fact apply to this situation.

Sorry again for any confusion.

JaMi



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http

Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread Abd ul-Rahman Lomax
At 07:09 AM 9/3/2003, Joe McCauley wrote:
I need to have a current return line with 3mm thickness. This line has a net
identifier of 'Iret'.
This line connects to a current sense resistor. I need to take a line from
this resistor to an amplifier input.
Here is what I understand from this: this circuit is measuring current by 
measuring the voltage drop across the sense resistor. The current being 
measured is sufficient that a 3 mm trace is required. Presumably the 
temperature rise calculations have been done Or the trace is that fat 
so that error due to voltage drop in the trace is minimized.

There is no need for this amplifier input line to be 3mm thick, in fact from
the point of view of routing it would be better if it were not!
Mr. McCauley writes about one line. Really, there are two, since one is 
measuring the voltage drop across a resistor. Of course, if there is a 
solid enough ground at the ground side of the sense resistor, one might 
assume that the drop in that part of the circuit can be neglected. Or 
perhaps the circuit will be calibrated to account for that additional drop. 
Otherwise one needs *two* sense lines, which will feed a differential 
amplifier of some kind.

Presumably there will be negligible current in the sense line (the 
amplifier input line.) At least whatever measures that voltage should be 
designed to minimize the current. So the line can be narrow, really it only 
needs to be wide enough to be reliably fabricated.

 Is there a
way of joining 2 different nets in the schematic while keeping seperate
identifiers? If there were then I could setup the design rules in PCB to
always have the 'Iret' net 3mm thick, while the other one which connects to
it could be (say) 0.35mm. Am I over complicating things by trying to do it
this way?
I don't think so. I'm from the school that thinks that good DRC is very 
important. You can certainly accomplish what you want by setting the 
minimum thickness for Iret at 0.35 mm and the maximum at 3 mm. But this 
won't guarantee that you get 3 mm where it is needed.

There might be some way to do this with from-tos, as mentioned by another 
designer, but I don't know that. I do notice that From-To Class is one of 
the possible attributes controlling width rules, but I've never 
investigated that rule. Maybe I should read the manual Naah, that's 
something I recommend to others, I don't do it myself :-)

As mentioned by Mr. Ross, the so-called virtual short will accomplish 
this. Once you have built this footprint, have placed a symbol for it on 
the schematic and have wired it, and have set a design rule for the 
footprint (or component class, if by some chance you had different kinds of 
these creatures), it is pretty much set and forget.

You would have your IRet net, being the return net for your large current. 
Then you would place, on your schematic, the virtual short, which is, for 
schematic purposes, a jumper. One side of the jumper is connected to IRet, 
typically right at the sense resistor pad. The other side of the jumper is 
connected to your sense net that goes to the amplifier. You could actually 
make the jumper structure part of the sense resistor pad, which would 
guarantee that the short is placed in the proper location. In other words, 
you'd build a symbol and footprint for the sense resistor that had two 
extra pads for the sense connections.

These pads have a gap between them which is below fabrication possibility. 
Properly designed, there will actually be *no* gap on the films, because 
the gap will be well below the gerber resolution. It might be, say 4 
microinches. (Protel can get a tad flaky in the microinch region since 
that's the database resolution, as I recall, otherwise it could be 1 
microinch!) Then a design rule allows pads in that particular footprint to 
be very close to each other, say 2 microinches, without creating a DRC 
violation. By the way, you'll use rectangular pads

How do you make the virtual short? I described above the principle for 
using fabrication limits to create a physical short that Protel considers 
as being unconnected. There is at least one other way, which became 
practical and reasonably safe when the CAM Manager was created, allowing 
custom CAM setups for your design. One of the mech layers is dedicated to a 
short, that is, a shorting trace is on that mech layer. It is merged with 
the normal layer as part of the CAM definition for the normal layer.

With the fabrication limit method, you need to create a design rule. It's a 
good thing that if you forget to do this, you will get a DRC error, so this 
is quite safe. The down side of this method is that if you aren't careful 
about how your CAM pad definitions are created, roundoff can leave a real 
gap on the film and a helpful fabricator will increase it for you, this has 
actually happened. The mech layer merge technique will produce a 
bulletproof fab film, but if you forget to create the CAM definition 

Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread JaMi Smith

- Original Message -
From: Abd ul-Rahman Lomax [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, September 03, 2003 4:50 PM
Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers?


 At 07:09 AM 9/3/2003, Joe McCauley wrote:
 I need to have a current return line with 3mm thickness. This line has a
net
 identifier of 'Iret'.
 This line connects to a current sense resistor. I need to take a line
from
 this resistor to an amplifier input.

 Here is what I understand from this: this circuit is measuring current by
 measuring the voltage drop across the sense resistor. The current being
 measured is sufficient that a 3 mm trace is required. Presumably the
 temperature rise calculations have been done Or the trace is that fat
 so that error due to voltage drop in the trace is minimized.

 There is no need for this amplifier input line to be 3mm thick, in fact
from
 the point of view of routing it would be better if it were not!

 Mr. McCauley writes about one line. Really, there are two, since one is
 measuring the voltage drop across a resistor. Of course, if there is a
 solid enough ground at the ground side of the sense resistor, one might
 assume that the drop in that part of the circuit can be neglected. Or
 perhaps the circuit will be calibrated to account for that additional
drop.
 Otherwise one needs *two* sense lines, which will feed a differential
 amplifier of some kind.

 Presumably there will be negligible current in the sense line (the
 amplifier input line.) At least whatever measures that voltage should be
 designed to minimize the current. So the line can be narrow, really it
only
 needs to be wide enough to be reliably fabricated.

   Is there a
 way of joining 2 different nets in the schematic while keeping seperate
 identifiers? If there were then I could setup the design rules in PCB to
 always have the 'Iret' net 3mm thick, while the other one which connects
to
 it could be (say) 0.35mm. Am I over complicating things by trying to do
it
 this way?

 I don't think so. I'm from the school that thinks that good DRC is very
 important. You can certainly accomplish what you want by setting the
 minimum thickness for Iret at 0.35 mm and the maximum at 3 mm. But this
 won't guarantee that you get 3 mm where it is needed.

 There might be some way to do this with from-tos, as mentioned by another
 designer, but I don't know that. I do notice that From-To Class is one of
 the possible attributes controlling width rules, but I've never
 investigated that rule. Maybe I should read the manual Naah, that's
 something I recommend to others, I don't do it myself :-)

 As mentioned by Mr. Ross, the so-called virtual short will accomplish
 this. Once you have built this footprint, have placed a symbol for it on
 the schematic and have wired it, and have set a design rule for the
 footprint (or component class, if by some chance you had different kinds
of
 these creatures), it is pretty much set and forget.

 You would have your IRet net, being the return net for your large current.
 Then you would place, on your schematic, the virtual short, which is, for
 schematic purposes, a jumper. One side of the jumper is connected to IRet,
 typically right at the sense resistor pad. The other side of the jumper is
 connected to your sense net that goes to the amplifier. You could actually
 make the jumper structure part of the sense resistor pad, which would
 guarantee that the short is placed in the proper location. In other words,
 you'd build a symbol and footprint for the sense resistor that had two
 extra pads for the sense connections.

 These pads have a gap between them which is below fabrication possibility.
 Properly designed, there will actually be *no* gap on the films, because
 the gap will be well below the gerber resolution. It might be, say 4
 microinches. (Protel can get a tad flaky in the microinch region since
 that's the database resolution, as I recall, otherwise it could be 1
 microinch!) Then a design rule allows pads in that particular footprint to
 be very close to each other, say 2 microinches, without creating a DRC
 violation. By the way, you'll use rectangular pads

 How do you make the virtual short? I described above the principle for
 using fabrication limits to create a physical short that Protel considers
 as being unconnected. There is at least one other way, which became
 practical and reasonably safe when the CAM Manager was created, allowing
 custom CAM setups for your design. One of the mech layers is dedicated to
a
 short, that is, a shorting trace is on that mech layer. It is merged with
 the normal layer as part of the CAM definition for the normal layer.

 With the fabrication limit method, you need to create a design rule. It's
a
 good thing that if you forget to do this, you will get a DRC error, so
this
 is quite safe. The down side of this method is that if you aren't careful
 about how your CAM pad

Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread JaMi Smith
Oops, sorry for the empty response . . . that's what happens when you double
click the reply button . . . operator error . . .

I think that there should be a little more clarification of a few things
before the misunderstanding in this thread becomes too rampant.

There are basically two different ways that a current sense resistor is
normally used. The first is between a voltage source and a load, and the
second is between the load and ground. In both cases, the voltage drop is
measured across the current sense resistor between the supply leg and the
load.

Typically, in this type of scenario, the voltage source is the output of a
regulator, with the feedback from the load side of the current sense
resistor being used to control the output of that regulator.

My original response and follow-up, as well as my response to Ian's post,
are based on a current sense resistor being used between the voltage source
and the load.

I believe that Ian's response to my post also assumed that we were talking
about the current sense resistor being placed between the voltage source and
the load also, but it may not have, although it does not really make a
difference in his post or in my response to it.

It appears that Abd, in his response below, is invisioning the current sense
resistor in the second location mentioned above, which is between the load
and ground, or possibly that could be better understood if it is stated as
the between the return from the load and the ground. While this is
different than I envisioned, the problem is really the same, and that is
that the current sense resistor is usually put in one leg of a supply or
regulator curcuit (either positive or negative) so that the current can be
determined by measuring the voltage drop across the resistor between that
leg of the supply and the load, or if you prefer, between the load and
the supply.

In either case, the feedback to the amplifier must be connected to the
load side of the current sense resistor, with the other side of the
current sense resistor connected to the appropriate positive or negative
source, as dictated by the design requirements of the circuit, such that the
current sense resistor is in series with the load

This load side of the current sense resistor is both the place that any
high currents going to or comming from the load must travel in order to
get from or to the supply (or regulator circuit), and it is also the place
from which a feedback trace must be connected back to the input of the
amplifier that moniters the voltage drop across the current sense resistor.

I am pointing this out so that anyone reading this compilation of responses
can understand the differences in the possible location of the current sense
resistor in the different discussions, and understand that while there are
these differences, the requirements for handling the feedback from the
load side of the current sense resistor is virtually the same in all of
the discussions, notwithstanding possible confusion brought about by where
the supply end of the current sense resistor is located.

With that said, I have a few additional comments below.

JaMi

- Original Message -
From: Abd ul-Rahman Lomax [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, September 03, 2003 4:50 PM
Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers?


 At 07:09 AM 9/3/2003, Joe McCauley wrote:
 I need to have a current return line with 3mm thickness. This line has a
net
 identifier of 'Iret'.
 This line connects to a current sense resistor. I need to take a line
from
 this resistor to an amplifier input.

 Here is what I understand from this: this circuit is measuring current by
 measuring the voltage drop across the sense resistor. The current being
 measured is sufficient that a 3 mm trace is required. Presumably the
 temperature rise calculations have been done Or the trace is that fat
 so that error due to voltage drop in the trace is minimized.

 There is no need for this amplifier input line to be 3mm thick, in fact
from
 the point of view of routing it would be better if it were not!

 Mr. McCauley writes about one line. Really, there are two, since one is
 measuring the voltage drop across a resistor. Of course, if there is a
 solid enough ground at the ground side of the sense resistor, one might
 assume that the drop in that part of the circuit can be neglected. Or
 perhaps the circuit will be calibrated to account for that additional
drop.
 Otherwise one needs *two* sense lines, which will feed a differential
 amplifier of some kind.

 Presumably there will be negligible current in the sense line (the
 amplifier input line.) At least whatever measures that voltage should be
 designed to minimize the current. So the line can be narrow, really it
only
 needs to be wide enough to be reliably fabricated.


I would disagree here, in that I believe that the trace should be large
enough to not contribute any losses of its

Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread Ian Wilson
On 12:43 PM 4/09/2003, JaMi Smith said:
There are basically two different ways that a current sense resistor is
normally used. The first is between a voltage source and a load, and the
second is between the load and ground. In both cases, the voltage drop is
measured across the current sense resistor between the supply leg and the
load.


I think, Jami, that you are missing a critical aspect or it is getting 
buried in too much verbage. Sorry if I have just missed it, I am afraid I 
am doing you something of a disservice by not reading your post(s) in full.

It is common to have four connections to a current sense resistor, two on 
each side.  One on each side will be big and fat to carry the current, and 
the other with be a signal trace (carrying no current) that ensures the 
voltage drop across just the resistor is sensed - the voltage drop across 
power tracks, ground planes etc are ignored.  The only tricky stuff with 
this is that it requires common-mode input ranges beyond, or at least close 
to, the supplies in many situations - but this is no longer rocket science.

Ian



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread Thomas


 -Original Message-
 From: Ian Wilson [mailto:[EMAIL PROTECTED]
 Sent: Thursday, 4 September 2003 13:11
 To: Protel EDA Forum
 Subject: Re: [PEDA] Joining 2 different nets keeping seperate
 identifiers?
 
-snip-
 
 I think, Jami, that you are missing a critical aspect or it 
 is getting 
 buried in too much verbage. Sorry if I have just missed it, I 
 am afraid I 
 am doing you something of a disservice by not reading your 
 post(s) in full.
 
-snip-

I hear that.
If I had time to read Jami's posts in full I would not be at work! :)


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread JaMi Smith

- Original Message -
From: Ian Wilson [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, September 03, 2003 8:10 PM
Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers?


 On 12:43 PM 4/09/2003, JaMi Smith said:
 There are basically two different ways that a current sense resistor is
 normally used. The first is between a voltage source and a load, and
the
 second is between the load and ground. In both cases, the voltage drop
is
 measured across the current sense resistor between the supply leg and the
 load.


 I think, Jami, that you are missing a critical aspect or it is getting
 buried in too much verbage. Sorry if I have just missed it, I am afraid I
 am doing you something of a disservice by not reading your post(s) in
full.


You are right in that sometimes I can get too longwinded in trying to
explain someting, and I really need to try and just keep it short and
simple.

 It is common to have four connections to a current sense resistor, two on
 each side.  One on each side will be big and fat to carry the current, and
 the other with be a signal trace (carrying no current) that ensures the
 voltage drop across just the resistor is sensed - the voltage drop across
 power tracks, ground planes etc are ignored.  The only tricky stuff with
 this is that it requires common-mode input ranges beyond, or at least
close
 to, the supplies in many situations - but this is no longer rocket
science.


I agree with most here except the carrying no current, where I would say
that that there is quite probably at least a small amount current (unless
the amplifier has CMOS or FET inputs) but which is nontheless large enough
to be affected by the restivity of the trace, where too narrow a trace, or
differences in thickness and or width in manufacturing could cause
differences in operation of the sensing circuit from board to board. If this
is a very high current application, there could even be some fairly decent
currents in the feedback loop, depending on just what was going on in the
regulator portion of the circuit. In many regulator IC's this feedback
input can even be the base of a bipolar transistor, whose operation is
actually current controlled, notwithstanding that it may appear an amplifier
in the datasheet. Even in the case of CMOS or FET inputs to an amplifier,
which I think would be avoided in this type of application, but which really
would have no current flow involved, I would still maintain that crosstalk
and any losses due to restivity should still be avoided.

I concurr respecting the 4 connections, but I am simply assuming that the 2
connections on the side of the voltage source (or ground in the sceneario
discribed by Abd) are considersd internal to the regulation circuit, and
have therefore not discussed them.

I am also assumming that there is a regulator circuit involved in the
original application which lead to the initial questions in this post, but
possibly I am going to far in that assumption, which I have based most of my
comments on, and even some here above. Oh well.

Thanks for the feedback.

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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread Abd ul-Rahman Lomax
At 10:43 PM 9/3/2003, JaMi Smith wrote:
[in the original inquiry it was stated:]
 I need to have a current return line with 3mm thickness.
return generally refers, in my experience, to the wiring which returns to 
ground or other more negative voltage. I'm sure someone can come up with a 
more precise definition. But it might be used, in this case, to refer to 
the return line coming from the load, not to ground, but to a sense 
resistor and from there to ground or common. The sense resistor is of a low 
value, and the voltage drop created by the current through it will be small 
compared to the voltages involved in driving the load.

[...]
 This line connects to a current sense resistor. I need to take a line
from
 this resistor to an amplifier input.
The writer did not state which side of the resistor is connected to the 
amplifier input. The imprecision of the question has led to a bit of 
confusion in the answers, but it does not really affect the most important 
part of the answer, only the dicta.

Since the writer only refers to one sense line, I'm assuming that the 
voltage drop in the current path from the resistor to ground may be 
neglected; otherwise one would need to use *two* sense lines and a 
differential amplifier, though it might also be possible to calibrate the 
circuit and get away with only a single sense line. In other words, the 
true sense resistor would be the assembled part plus the resistance of the 
remainder of the ground circuit.

Quite clearly, however, the inquirer was concerned with a voltage sense 
line and its different width requirements from what is otherwise the same 
net, Iret. Perhaps the amplifier is located on the other side of the 
circuit board, or even on another circuit board.

[I wrote:]
 Presumably there will be negligible current in the sense line (the
 amplifier input line.) At least whatever measures that voltage should be
 designed to minimize the current. So the line can be narrow, really it
only
 needs to be wide enough to be reliably fabricated.

I would disagree here, in that I believe that the trace should be large
enough to not contribute any losses of its own by being so narrow that
differences in manufacturing runs may produce traces which may have
differences in their own resistivity, which will in fact affect the circuit.
Mr. Smith must be having a bad day. (Or I've really lost it myself, 
certainly  a possibility)

The resistivity of this line in a current measurement application will have 
no effect on the voltage at the amplifier, since, in a properly designed 
circuit, there will be no current in the trace. If there is no current, 
there is no voltage drop. True, if the current is rapidly varying, 
resistance could create some problem, but it would be unlikely in a normal 
power application for this to be an issue.

There needs to be a good direct path from the load side of the current
sense resistor back to the input of the amplifier, and it needs to have no
problems of its own such as losses or crosstalk from other circuits.
Crosstalk might be an issue, I suppose, but, again, in power circuitry, it 
would be unusual for the problem to be such that a bit of capacitance at 
the amplifier input would not eliminate it. We might be talking DC, here. 
If crosstalk is an issue, I'd think the thickness of the trace might be 
irrelevant If we are talking RF, all bets are off.

Assuming that Iret is in fact the return net from the load,
Yes, I'm sure that's what he meant. He's free to chime in with a 
correction, of course!

 and is a
large trace connected to one end (the load end) of the current sense
resistor, with the other end of the current sense resistor being connected
to ground (the negative supply),
Yes. It's a large trace for heat reasons, less likely losses might be an 
issue. But losses in the Iret trace will not affect the current measurement 
if the sensing point is right at the high end of the sense resistor.

Drop in the ground end net *would* be an issue, though it might be possible 
to ignore it, as was implied by the question.

 I would say that there should be another
trace going from the same Iret end of the current sense resistor to the
amplifier input.
Another trace? That's the trace he was asking about!

Perhaps Mr. Smith intended to refer to a trace from the ground end (not the 
Iret end) of the sense resistor, which would then be used in a 
differential voltage measurement, i.e., a differential amplifier would be 
used. But this was not the question we were asked. However, the trace size 
and naming and DRC issues would be the same, only it would be with two 
traces instead of one.

 This trace is the feedback portion of the Iret trace,
or what I would call the feedback trace, but there is absolutely no reason
in the world that this trace should have a different net name, or have any
virtual short involved with it.
I must say that Mr. Smith has lost me here. feedback? Feedback would be 
involved in the amplifier 

Re: [PEDA] Joining 2 different nets keeping seperate identifiers?

2003-09-03 Thread Abd ul-Rahman Lomax
At 11:10 PM 9/3/2003, Ian Wilson wrote:
It is common to have four connections to a current sense resistor, two on 
each side.  One on each side will be big and fat to carry the current, and 
the other with be a signal trace (carrying no current) that ensures the 
voltage drop across just the resistor is sensed - the voltage drop across 
power tracks, ground planes etc are ignored.
They are ignored because they are irrelevant. This kind of arrangement is 
used with some kind of differential amplifier (or bridge, I suppose), so 
the current will be equal to the differential voltage divided by the sense 
resistance, quite accurately, it will be as accurate as the resistance.

However, in some circuits it might be possible to ignore the ground leg 
drop. For example, the ground connection might be through a ground plane, 
and the sense amplifer circuitry is referenced to this same plane I'm 
not describing all the details and possibilities... (do I hear a sigh of 
relief? :-)

  The only tricky stuff with this is that it requires common-mode input 
ranges beyond, or at least close to, the supplies in many situations - 
but this is no longer rocket science.
Normally the sense resistor, as I've seen it, is in the return, as in the 
matter at hand. So if, for example, we have high voltage to the load, we 
don't need to deal with high voltages in the current-measurement circuitry, 
we are only dealing with voltages close to ground, well within the 
instrumentation supply voltage. Of course, if the fabricator opens up that 
virtual short, we're likely to have a fairly spectacular error indication



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *