This user manual
briefly introduces the user to the four kinds of spirals that can be tested in
this program. The four spirals are listed below and a typical case in each is
explained below. The output the Spice
model is also discussed.
· Single and multi-layered inductors
·
Stacked transformer with primary in one layer and the secondary in
another layer.
· Interwound transformer with primary and secondary on the same layer.
· Stacked-interwound with primary and secondary turns equally divided between the two layers. It is the combination of stacked and interwound type transformer and has the best of both.
Explanation of the Spice model outputs
This subsection walks the user through a typical case for an inductor simulation and explains in detail each prompt. When the program is executed by typing in the Spiral at the prompt the following screen appears. The prompts from the program are shown in italics.
***********************************************************************
Inductor
0
Transformer
Stacked 1
Transformer
Interwound 2
Transformer
Interwound & Stacked 3
***********************************************************************
Enter a number from above (0) :
Figure
1: screen shot for input
It
gives an option to the user to choose the kind of spiral under test. The
default is an inductor and can be chosen by pressing enter or entering the
value 0.
Once
the type of spiral is chosen, the program prompts the user to enter the
technology data of the process. The data can be either read directly from a
preformatted data file or entered at the prompt. If the technology file does
not exist and the tech parameters need to be entered, then at the prompt type
‘no’. The program will prompt for the
different technological parameters such as the substrate specifications and the
layers’ properties.
Do u want to read tech data from file (yes)
: no
*************************
Substrate Specifications
*************************
Enter the value of epi thickness in microns
(2.0)
:
Enter the value of epi Resistivity in ohm_cm (5) :
Enter the value of substrate Resistivity in ohm_cm
(20) :
Enter the value of Shield to Ground Resistance in
ohms (1)
If No Shield, enter Substrate to Ground
Resistance :
Figure 2: Screen shot of substrate specifications
The program prompts for the substrate specification and the first specification is for the epi-layer thickness, which is typically between 2 to 5 microns. If the process does not contain any epi-layer the user can get around it by entering a value 0 for it. In the case the user enters a non-zero value for the epi-thickness the program prompts for epi-layer resistivity. The substrate resistivity in ohms-cm is prompted next. The value of that typically varies from 0.02 to 20 in normal CMOS process and much higher in SOI process. The default is set to 20 ohm-cm. Then the user is prompted for the shield to ground resistance. The shield is discussed in a moment. If no such shield exists, then enter the substrate to ground resistance. This value is output to the spice file, and has a large effect on the inductor’s Q. It has no effect on this program’s resistance calculations.
If the user does not know the value of a particular parameter, the default value, which is typical, can be entered. Once the substrate specifications are entered, the user is prompted for Shield specification. The shield is a low resistance material, usually the lowest layer of metal or poly, which is grounded and placed under the inductor to provide a low resistance path for the capacitive coupling, which in other case would have gone through a higher resistance substrate. To prevent the creation of large eddy loops, the shield is patterned, broken into several small pieces. The shield, which is also called ground plane in literature, is optional and may be avoided by typing ‘no’ when the program prompts for shield. However it seen that in medium and high resistivity substrate process the shield is very often used. In this case ‘yes’ is entered and the program prompts for the shield specifications.
Do u want a Pattern Poly Shield/ground Plane(no) : yes
*************************
Shield Specifications
*************************
Enter the value of Shied Thickness in microns (1.0) :
Enter the value of Shied Resistance in ohm/Sq (1) :
Enter Insulator thickness below shield in microns (1.2) :
Enter the value of Insulator Permitivity (3.9)
:
Figure 3: Screen shot showing the Shield specifications
If the user decides to use a shield, the program
prompts for the different shield specifications. First it prompts for the
shield thickness, which is the thickness of the layer, used as shield. The
shield resistance in ohms/sq is prompted next, which is again the sheet
resistance of the layer used. Then it prompts for the insulator thickness and
insulator permativity. As it is obvious from the name, the insulator thickness
is the separation between the shield and the substrate or to the epi-layer as
the case maybe. Next enter the
insulator’s permativity, the dielectric constant of the material. The default value is 3.9, the permativity of
silicon.
Figure 6 presents a typical layout of an inductor using a ground shield. In this case, the shield is made of n-type diffusion, and is surrounded by aground ring composed of n-diff, metal1, metal 2 and metal3. Metal 4 is used to jump over the ring.
Figure 4: Inductor layout with a shield and ground ring
The program
then prompts the user for the number of layers. It is the number of metal
layers used to make the spirals and not necessarily the total number of layers
available in the process. If a two-layered inductor is used with metal layers 1
and 3, the user types in 2 at the prompt for a number of layers. And in the
layer specification the metal thickness is entered in microns and the
metal resistivity in ohms / sq . In the
case of dielectric thickness, the user needs to enter the insulator thickness
between layer1 and layer3, the ones which are used for the spiral.
This program does not support vias with non-zero resistance connecting the different layers. It assumes the vias have zero resistance and also does not calculate the effect of the cross under trace. The inductor is assumed to be a perfect, squared layout. If they are deemed significant, the user may wish to tally up these excluded resistances and add a single, series resistance into the spiral.spice model file.
This paragraph explains with an example how the user
can model for sandwiched layers to get the benefits of higher sheet resistance.
An example would be a user who wants to simulate a two-layer inductor in a six-layer
process with a couple of layers sandwiched, and intends to sandwich 6,5 and 3,2
&1 to form his two-layer inductor. When prompted for the number of layers
the user would still enter the value 2. And in the layer specifications, for the lowest layer of metal
resistively the user would enter the value which is the parallel combinations
of the layers 1,2 and 3. For the insulator thickness, the distance between the
layer1 to the substrate should be entered followed by its permativity. For the
top layer specification, the parallel combinations of resistivities of layers 6 and 5 is entered metal resistivity. In
the same way the insulator thickness would be the separation between the layers
5 and 3.
The user may reuse this technology file by saving it
in the default.tech file or any other name of his choice. When running this
program again, the user can read the tech data from the file directly without
reentering the technology data again.
In this case a single layer spiral shown. So the program prompts for the one and lowest layer specifications as shown below.
Layer 1(lowest) Specifications
***********************************
Enter the value of metal thickness in microns (1.0)
:
Enter the value of metal resistivity in ohms/sq (0.04)
:
enter the value of dielectric thickness in microns (0.8) :
Enter the value of dielectric permativity (3.9)
:
Do You want to save tech data in file(yes)
:
Enter the name of the file(default.tech) :
Technology Data Stored in default.tech
Figure 5: Screen showing the different Layer specifications
Once the technology data is entered, the user is prompted for the geometry of the spiral. Figure 5 demonstrated the various parameters. First it prompts for the outer dimension, the physical outer edge to edge. It’s the same in case of multi turn spirals too. Then it prompts for the number of turns. In the case of single layer inductor, it’s the total number of turns, while for a multi-layered spiral it’s the number of turns on a layer. In the case of transformers the number of turns is the total number of turns of the primary winding. Even if the transformer has multiple layers, always input the total number of primary turns. The program assumes that primary and secondary are identical. The program then prompts for the width of the trace, which is the same for all turns. The next prompt is the pitch of the spiral. In the case of an inductor it is the center-to-center distance between the adjacent turns, or the width of the trace plus the spacing between the traces. In the case of transformers it’s the distance between the adjacent turns, i.e. the primary and secondary.
Figure 6: Single layer simple spiral inductor
Figure 7: Two
layer inductor, in on metal 2||1, out on metal 4 (yellow)
If you entered values for pitch and the number of
turns that would create a spiral larger than the given outer dimension, the
number of turns is adjusted. The programs calculates the maximum number of
turns possible and a new, adjusted outer dimension and outputs this to the
screen. The adjusted outer dimension
will never be larger than that size allocated at the input. It then calculates the rest of the
parameters and outputs it to a spice file. The calculated inductance and total
series resistance are also output. The spice file can be simulated using spice3
and the spiral characterized using standard techniques.
**************************************************
Geometry Specifications
**************************************************
Enter the Outer Dimension in microns
:350
The Number of Turns is
:4
The Width of the trace in microns
: 20
The Pitch between the traces in microns : 25
Figure
8: Screen shot showing the Geometry specification
The output is shown below for our particular case
after the program is simulated. It shows the total inductance and the total dc
resistance of the spiral.
The New Outer dimension is : 350
The New Number of Turns is : 4
Computing self and mutual inductances ......
Output of Spice model written to inductor.spice
Output of Spice main file written to spiral.spice
The Total Inductance 6.09671e-09
The Total Resistance 8.8
Figure
9: Screen shot showing the results after simulation
This particular geometry of transformer has primary in one layer and the secondary in the other layer. In this thesis only the case where the number of turns of primary and secondary are equal is dealt with. Figure 10 shows a common stacked design using a three metal process where it shows the secondary is on top of the primary. One layer conatins the primary, another the secondry, and the third layer is used to tie to the center nodes.
Figure 10: Stack transformer layout.
The advantage of this geometry is that it has a good coupling coefficient, however it suffers from very high capacitive coupling between the primary and secondary. The result is a very low SRF which makes it non-operational below the frequency of interest
In the following paragraphs an attempt is made to walk through the
different prompts and explain them. The user starts by typing spiral at the
prompt.
The screen as shown in Figure 1 comes up and the user can select the
transformer stacked by enter the value 1. As discussed earlier in section 6.1 the program prompts for the
technology file. The parameters are the same but with the exception that the
program does not prompt for the number of layers. As this geometry has two
layers, the program next prompts for the individual layer specifications. There
are the same as explained in section 6.1.
**************************************************
Geometry Specifications
**************************************************
Enter the Outer Dimension in microns : 350
The Total Number of Primary Turns
: 4
(if wound in then back out, it’s the TOTAL primary)
The Width of the trace in microns
: 20
The Pitch between primary and secondary in microns : 25
The New Outer dimension is : 350
The New Number of Turns is : 4
Computing self and mutual inductances ......
Output of Spice model written to transformer.spice
Output of Spice main file written to spiral.spice
The Total Inductance of primary or secondary 2.43868e-08
The Total Resistance of primary or secondary 17.6
Figure 11: Screen shot showing the geometry specifications and the result
In the geometry specification, the program prompts first for the outer
dimension of the transformer as shown in Figure 8. The value entered is in
microns. Then it prompts for the total number of turns on the primary
coil. The primary and secondary are
assumed to be identical. Then it
prompts for the width of the trace followed by the pitch. The pitch mentioned
in the transformer is the distance between the adjacent turns.
The output is written to transformer.spice and the spice main file to spiral.spice. The total inductance and resistance of primary or secondary is calculated and output to the screen.
This geometry of transformer has the primary and secondary in the same layer. As discussed in section 6.2 , the primary and secondary have the same number of turns. The primary and secondary follow each othe side-by-side around the spiral. As explained in the previous sections in this chapter the program starts with the screen as shown in Figure 1 when the user runs “spiral”. The technology file parameters are the same as in section 6.2 with the exception that the program assumes the number of layers as one and doesn’t prompt for it.
Figure 12: Typical interwound transformer layout
In the geometry parameters it prompts for the outer
dimension in microns first, followed by the number of turns. Once again, this
the total number of primary turns. The
width is the width of the primary or secondary trace. In this geometry of
transformer the primary and secondary traces are identical. The pitch is the
distance between the centers of adjacent primary and secondary.
This transformer has an innovative design geometry and uses the best of both worlds. The transformer discussed in section 6.2 suffers from the SRF problem and the one in section 6.3 suffers from low coupling. This geometry is an amalgamation of the transformers discussed in section 6.2 and 6.3. It has half the primary winding on one layer and the other half in the second layer. The same is the case with the secondary winding too. So it has a better coupling coefficient than the transformer of section 6.3 and much higher SRF than the simple stacked transformer. The capacitance between the primary and secondary is very negligible as compared to the stacked transformer.
The dimensions are entered the same as before. Use the number of total primary turns and the pitch is the
distance between adjacent primary traces.
Figure 13 shows a typical layout of am interwound-stacked transformer. Here, the primary resides in metal4, while the secondary uses metal2 paralleled with metal1. Notice how the two winds only overlap at the left corners.
Figure 13: Layout of a interwound, stacked transformer
This section introduces the
different spice files generated after running the program. In the later part it
also explains the parameters that need to be modified to run a simulation and
determine the other parameters.
All the four cases of
spirals when simulated generate two spice files. There is a model file which stores the model details
and the other file called the main file instantiates the model and contain the
control parameters for the simulation. The main file is the same in all the
cases and is called spiral.spice. In the case of inductor, the model file is
called inductor.spice. It is modeled as a spice sub-circuit with three output
terminals, which are visible to the user. The two terminals of the inductor and
the third terminal for the substrate or the shield connection form the three
terminals. In the case of all three
transformer models the model file is transformer.spice. Like the case of
inductor the transformers are also modeled as spice sub-circuits with five output terminals. The two terminals for the
primary and the two for secondary with the substrate connection form the five
output connections.
The spiral.spice file contains the control information to simulate it in spice. The inductor model is instantiated in this file. The three terminals of the inductor are called the inner_turn, outer_turn and the sub or shield depending on substrate or the shield connection.
Doing a frequency analysis and
sweeping in frequency from 0.1 GHz to 100Ghz characterizes the spiral. For
this, one terminal of the inductor is connected to a one-amp current source and
the other connected to ground. Note the
netlist line representing the shield (or substrate) to ground resistance. This
resistance affects the Q of the spiral where the eddy losses in the substrate
are not significant. In the case of absence of a shield, the substrate should
be connected to a suitable potential. Plotting the node “inner_turn” will provide the impedance graph versus
frequency.
In the case of a transformer, the five connection points are primary1, primary2,
secondary1, secondary2 and substrate. Again, a one-amp current source is connected to the primary. Plotting node “primary2” will provide nice
impedance curve from 10MHz to 100GHz
This model can be simulated in a spice3 program by running the spiral.spice
file. The results could be observed by plotting the different nodes. The SRF
and Q at SRF can be calculated from the graphs. To calculate Q at any lower
frequency a resonating capacitor can be used.