Q1: How can I make my working sheet large enough
to draw a big schematic?
You can redefine the page size using the function tool "Define page outline as
rectangle" from Edit/Page format menu item. Select this function tool and click
on the graphics area. You will get a window where the new page size may be selected.
Otherwise you may draw the rest of your schematic in a new page.
Q2: How can I stop the Bus member number
sliding, when I delete a net, that is bus connected with a defined bus number? I wish that
the other nets in bus hold their previously defined bus member numbers.
If you are deleting the whole net by selecting the function tool "Delete whole
net", then on redrawing the circuit the bus member number also gets renumbered. This
is because on deleting a net, the part once again gets repacked and it renumbers the bus
members also.
More on Bus member number
Bus member number allows to group nets having the same bus member number, So it is
advisable to have default numbers (0,1,2...). If the default bus member number (e.g. 0) is
to be changed, then select Recover net/ Bus labels and click on the bus member number. In
the window, enter the required name (D0) and click O.K.. Now click on all the bus member
number having the same bus member number (0) and assign D0.
On the other hand, if the Net name (NET1) is to be changed , then select Edit Nets
function tool in the Edit/Nets mode and click on the net name. In the pop up window,
change the name (NEW NET1). Now you will find that all the net having the same net name
(NET1) will be changed to the new name (NEW NET1).
Related topics
Recover Net/bus label text
Purpose: This option allows to Recover Net/ Bus label text & Bus member number
and also allows to edit Bus name, Bus member number and Net name.
Operation:
To recover
Net name click on the wire nearer to the node. Bus member number: click on the wire nearer
to the bus. Bus name: click on the bus.
The recovered text get tagged to the cursor. Now place this text just below the wire from
where it is recovered inorder to avoid confusion.
To edit
Net name:Click on the net name and enter the new name in the window that opens.
This method of change is not advisable because all the nets having the same name should
also be changed to the new name.
Inorder to avoid confusion net name may be changed by using the tool Rename existing net
or text edit new net invoked from Edit/Nets which changes all the nets having the same
name, then the net name may be recovered using Recover Net/ Bus label text tool.
Bus member number: Since this number allows to group nets having the same bus
member number, it is advisable to have default numbers(0,1,2...). If the default bus
member number(e.g. 0) is to be changed, select Recover net/ Bus label and click on the bus
member number. In the window, enter the required name(D0) and click O.K.. Now click on all
the bus member number having the same bus member number(0) and assign D0.
Bus Name: Click on the Bus name and edit it in the window that pops up OR Select
the option tool Rename bus and click on the BUS.
The ability to add board description notes to any layer was removed on purpose. This again
will create problems when generating Gerber files. It is for this purpose that we have
introduced Mechanical plot. This contains mechanical details of the file such as
dimensions and notes that are available on Comp. Print and Solder Print.
Rename Existing Net Or Text Edit New Net
Purpose:
While preparing the schematic diagram, a net may not be named according to its
functionality. Later it may be required to rename the net according to the function it
performs. This function tool may be used to rename an existing net.
Operation:
Select this function tool and click on the net to be renamed. A dialog box listing the
nodes and the present name of the net gets displayed. The name may be changed in the text
box Netname and to confirm the change click the "ACCEPT" button.
To recover the new net name select Recover net/bus label text function tool from Edit->
Traces.
Q3: In Schematic capture, after a circuit is
drawn , we autopackage Can you explain what is actually taking place in autopackaging and
why ?
The autopackaging utility allows to perform the automatic packaging of all unpacked
components and it assigns the first free number to the last placed components belonging to
the same group. The component Name prefixes from Part descriptions are used to
automatically generate component names.
When you actually autopackage, system extracts the package assigned to the part at the
time of creation. This is how it displays the respective package facilitating front
annotation.
Q4: Why do we need to specify the swap level
in the entry attributes? What difference it is going to make if it is given 1 or -1? And
why do we need visible pinout?
If Swap Level is set to -1, it will not allow the pin to be swapped. If it is set to 1 or
any positive integer, this means that the pin can be swapped with any other pin having the
same swap level. For e.g.: the input pins of 2NAND may have their swap level set to 1
since they may be swapped. But the output pin of 2NAND should have this swap level set to
-1. If you want view pinout after packaging, you can set the Visible Pinout option
i.e. it decides whether pinout should be displayed when packaging.
Q5: I autopacked a schematic and all four
opamps went into four separate IC's. Then on trying to get them into one IC, I find that I
cannot individually pack the op amps. How do I sort this out?
This could have happened in the following way:
For e.g.: LF147 contains four symbols OPAMP, OPAMPA, OPAMPA, OPAMPA. To load the part
LF147, Select the function Create Component to open the Create Component window. In
this window under part text box, LF147 will be displayed and in the symbol text box OPAMP
is displayed. When ACCEPT is clicked OPAMP is loaded. If this step is repeated again,
another OPAMP symbol will be loaded. Now packaging the symbols will load two ICs of part
LF147 in the layout. This is because part LF147 contains only 1 OPAMP. On the other hand,
if you select OPAMPA from the symbol dropdown list while loading the part LF147, and then
package, you will get only one IC in the layout since a single LF147 contains OPAMP and
OPAMPA.
The function tool Repack allows repackaging an already packaged component. Packaging of a
component is done according to the setting in the EDWin32 Main Menu Options/Packaging
Preferences. The three settings in the Preferences for packaging are Component name,
Description and Pinout details. Any or all of these can be set or removed. If you select a
packaged component, change the default settings of Packaging Preferences and try to
package it again, an error message appears saying "This component is already
packaged". So to package the component with the new details use Repackaging option.
Q6: EDWin32 concept of nets and wires
Net is a collection of nodes that are electrically connected together. A wire is merely a
visual representation of the corresponding net description. The creation of a wire
automatically results in the creation of the corresponding Net. Further, the deletion of a
wire removes only the wire but does not remove the Net whereas the deletion of a net
removes ALL the associated wires. The deletion of a node in the net removes the
corresponding connection in the net and removes the associated WIRE SEGMENT also.
It is possible to delete a wire and the corresponding net connection together by the
following procedure. From the Schematics Capture window select Edit/ Nets. Select
the 'Delete single Node' tool (shortcut *NN) from the vertical toolbar. Click on the
appropriate node. A confirmation box pops up asking to confirm the delete operation.
Select Yes to delete the node. This will delete the associated wire segment also.
Q7: How do you print the schematic hierarchy
contents?
To print the Schematic hierarchies, select the specific Schematic hierarchy from the list
of hierarchies and select Schematic Capture. Then Select Pages/Print Page to print
the schematic hierarchies.
Q8: How can you assign default pin number for
schematic in edit part?
You cannot assign default pin number for schematic in Edit Part. When a new entry is
created default pin numbers will be set by the system in the order of creation i.e. the
first (default) entry on screen will have pin number #1 assigned to it, the next one is
given the number #2 and so on. This will be displayed on screen if the option View
/Symbol/ Entry Number.
Q9:How do you change the thickness of wires?
The thickness of wires & buses can be changed even after routing.
1. Invoke Options /Sizes /Conductors from EDWin32 Main. 2. In the text boxes
provided for bus and wire line width, change the value to say .050.
Now to effect this change as default settings. Check Options-Default to current.
Note that if this change is just for the current database, then before changing the value,
check Options-Current and proceed with the above two steps.
Q10: When I use "redraw on
component" in Schematic, an error-message "component not found" appears
although the component is apparently there in the schematic and in the printout.
When you redraw a component in Schematic, specify the group of the symbol on which the
zooming operation is to be done, i.e. zoom on 7474/1 that is packaged as IC4 in the
schematic. Enter the name as IC4/1 in the input box that pops up when "Redraw on
Component" is selected. On the other hand when redraw on component is done in the
Layout, only the name IC4 is to be entered. Select tool "Display Component
Info" and click on any component in the schematic, the component name is given
along with the symbol group. This is the way the names are to be given when redraw is
done.
Q11: How can I make Pin numbers of a new
symbol visible in different Editors?
Load the symbol and check PA Texts from View menu. Position the PA Text and select the "Edit
Entry Attributes" tool. Now click on each entry and check the "Visible
Pinout" check box. This will display the pin numbers in the Schematic after the
component is packaged. Make all PA texts of a symbol visible/ invisible using Library
Viewer as follows:
In Library Viewer, Edit the symbol. In the dialog that pops up, check "EDIT PA SHIFT
" option button. Now click on any of the entries and click "ALL VISIBLE"/
"ALL INVISIBLE " button. Note that with both the methods it is necessary to save
the symbol after editing. In Library Viewer the "EXIT" button will be enabled
only after unselecting the entry by clicking in a vacant area. Also note that pin numbers
may be made visible in schematic only if the component is loaded as part.
Q12: About Merging and Splitting of Nets: I
am not able to split and also end up in merging the nets which I don't want to?
Splitting nets is a very simple process in EDWin32. Now say that you want to delete UN1.
Delete a wire segment. In Edit/ Nets mode, Select Split Nets function tool.
Click on the wire (UN1), the entire net gets selected. Click once again on the same wire,
this pops up a window, enter a new net name (system automatically inserts the first free
number) and check "Named " in the window. Accept the new net name and
verify using the tool Display Net info. To merge, select the net you want to merge and
click on the another net. A confirmation prompts. Now click YES to merge two nets into
one.
Caution: Before Splitting of nets, ensure that a wire segment is deleted.
Q13: How is a resistor, capacitor, inductance
etc. given a value and a power rating in schematic capture. In the file -res.part, what
does rc5a, res15w, rn50, rsip5 etc. mean in terms of component, value, power rating etc.?
The resistor/capacitor library was created based on resistance values coded according to
the MIL standard. The name of each resistor is formed by concatenating the IEC coded
resistance value with the corresponding package name. The MIL notation for values is as
follows:
In a 'N' digit value first (N-1) digits represent the significant figures and the last
digit represent the number of zeros to follow. The position of 'R' denotes the decimal
point.
For example 1001 -> 10000 (10K)
1002 -> 100000(100K)
2R7 -> 2.7
10R0 -> 10.0
That means the part 1000RC07 represents a 10K resistor using a RC07 layout. This was done
so that the schematic displays the values correctly after packaging but on the other hand
offered only a few layouts for the design. Now the resistor/capacitor library is
restructured according to the standard Sizes and wattages are available and a different
technique is designed for representing the values in the schematic. Also each part is
attached with a "Full Name" that gives a short description.
In EDWin32 there is a feature to add component values in schematics. For this you have to
select Edit /Components and select the function tool Add component text/Component
value(shortcut. *CT). They will appear on diagrams and component list (list of materials
editor).
Q14: I made the schematic diagrams and the
layouts for an audio pre-amplifier and amplifier in 2 different databases. Is it possible
to merge the two merge both diagrams and layouts to create one single schematic diagram
and layout?
You cannot make any link between two databases in EDWin32. The only way is to Block copy
one schematic into the other and paste it in the first database. And make necessary net
connections to work properly. This process is relevant for the Layout Editor also.
|