Q1: Please tell me if there is a
function in EDWin, where I can take a print out the library (all or a part of it).
You can print the list of parts; its associated Symbol, No. of groups of Symbol and
Package (name of component used), using the List Generator (Right click on the task, EDWin
XP/2000 in the Project Explorer to popup a list of functions). Click on List Generator in
this list to open up this module of EDWin XP/2000.
Q2: I would like a part library in the EDWin/ lib folder that is
recognizable by the EDWin parts to be available for the search list just as the other
supplied libraries.
Once you have created the parts, save the part in the library. Select the path (EDWin/ lib
if that is the path you need) and enter the new name of the *.PART file in the text box
(say MINE.PART) under the path selection box. Now click on SAVE. You can save all your new
parts to this new PART file. To include this newly created part file in the Search
sequence, select the View/ Search Sequence menu from the Library Browser/ Library Explorer
and check the files that have to be included in the Search list explicitly.
Q3: I built a simple schematic with IC's from the library that I
built. The problem is that when I tried to build a layout, the SLP1 & SLP0 net was not
connected to any of the ICs. I checked the parts everything looked just fine. Any idea
what's going on?
If you load ICs from the Library, it should have SPL1 and SPL0 nets already
assigned. You can see this in the Library editor window. For the part you created, you
should assign SPL0 and SPL1 explicitly for the pins, which are to be set as Gnd and Pwr
nets respectively, during creation in Editor. Load these to the Schematic, package them
and then invoke layout. Now you will get the ICs in the Layout. Select Info/ Nets to view
all the Nets that are already assigned. You should get SPL0 and SPL1 there.
Q4: I'm working on a layout where I need to arrange 15 LED's in
a circle, with equal distance between them.
Create a symbol as said below and load this as symbol in layout. First measure the LED
width between its two ends. Now create a line of that length and place it. Create a
contact point (Select point P1) to define the rotation of the line. Using the rotate and
repeat option tool click on the line. Enter the no of lines to be created and the angle
(360°/total no of the item). You see that you get a circle. Now relocate the default pad
(or change the pad) at one end of the line. And once again define the rotation by placing
a contact point. Click on the pad with the rotate and repeat option tool. Enter the same
value as above. Create another pad and place it on the other end of the line. Rotate and
repeat this pad as explained above.
Q5: Can I link one entry point of the symbol to more pads of the
package?
Assigning one entry point to more than one pins and vice versa is not possible with EDWin.
Q6: The problem of associating multiple layout pins to a single
schematic entry:
EDWin does not allow associating multiple layout pins to the same symbol entry. That means
if you have three V+ or V layout pins, you should create three schematic entries for
complete assignment. Otherwise you may create SPL0/SPL1 like Supply Pins net for the part.
For example you may create SPL_V+ and SPL_V by editing the Supply Pins while creating the
part. But both these methods are not satisfactory while attaching SPICE models or
subcircuits for the part as the subcircuit normally will have only one V+/V node. Now
there are two work around methods to solve this problem:
1) Create a symbol with three V+ nodes and three V nodes and complete the part. Now edit
the subcircuit file using a text editor to change the number of subcircuit nodes equal to
the number of entries of the symbol. You may have to add four more node numbers to the
.SUBCKT line for accounting two extra V+/V entries. Care should be taken to ensure that
the node numbers added do not conflict with the original node numbers. These newly added
nodes should be internally shorted inside the subcircuit. Now this subcircuit may be
adapted using Subcircuit Adapter linked with the schematic using EDSpice Symbol Editor or
EDSpice Simulator and simulated.
2) The second method is to create a symbol with only single V+ and V nodes and assign the
subcircuit straight away. But this results in "Unassigned entries/Entry mismatch
" error while creating part. Ignoring this error means that the unassigned layout
pins should be explicitly routed or these pins should be added to the V+/V netlist before
autorouting. There will be a warning " Symbol Entry missing " while routing the
trace/net that may be ignored.
The former method requires some knowledge about SPICE syntax; results in unconventional
schematic but is better suited if the layout of the design has to be produced. The latter
is an easier method but extra care should be taken for creating the layout of the design.
Q7: How can I assign simulation function to the symbol with 68
pins in order to edit it. If we can't assign with the same no. of pins , it implies that
we can't edit a new component with no. of pins that is not available in the library?
You can simulate only those parts that have a simulation primitive available for it. In
each version of EDWin, we keep adding new simulation primitives so that almost all parts
provided in Library will be simulated. These Primitives are functional level descriptions
of behavior of the simulated components. Executable code and data of the primitives are
placed in the Dynamic Link Library files (*.DLL) which are found in the EDWin Library
Directory. With these DLLs we define the input and output pins and these have to be
matched with that of the symbol while assigning the simulation function so that the
simulator can analyze the behavior of each pin.
If you create an entirely new symbol, you have two options:
If the symbol works like any other symbol for which a simulation primitive is already
available, you can assign the same primitive to it. If not, you will have to write the DLL
(simulation primitives) for simulating it and then assign it. The DLL primitive source
code is written in C programming language. The creation or updation of the primitives
requires some knowledge and practice with the C programming language.
For more details on writing the DLL, refer EDWin CD-ROM Primitives in Simulation/
Makeprims.doc.
Q8: The display of Packaging information is useful for ICs but
is confusing for resistors, capacitors etc. Is there any way to have only the information
needed?
Select Options/ Packaging Preferences from EDWin XP/2000 in the Project Explorer. In the
window, check off/on Comp.Name, Comp.Desc and Pinout as per your requirement.
Now you may repack the required components either selecting them individually (Tools/ Com
ponents Pack/Unpack component with option F2 selected) or in a block (Tools/ Block Edit
Unpack/Repack components in block with option F2 selected). These components will be
repacked according to the set preferences.
Q9: How can I avoid duplicating the parts already present in
Library, because I draw most of them myself and where can I find information regarding
case style encoding?
You can make a list for a particular library with part full name and keep this as a text
file for reference. For creating the list, invoke the List Generator by right clicking on
the task, EDWin XP/2000 in the Project Explorer. This text will contain all case styles
used in EDWin XP/2000 library.
Q10: When I choose a graphic tool a default shape is already
placed .How can I change the size and direction?
After placing the graphic tool on the board you have to stretch that particular item to
the required size using the tool ‘Stretch Item’ from the toolbar. Do remember
the zoom size value. If you want to create a graphic item from the scratch with a required
size then create the graphic items using the place contact points and then select the
particular graphic tool and click on the workspace.
Q11: How can I find dimensions?
1. You can view the dimensions of graphic items using the tool "Create items using
text " from the toolbar. In the pop up window you can view the properties of the
graphic item selected.
2.Another method for measuring the dimensions of graphic item is by setting the reference
point. Switch on Preference/-Ref Point and keep the cursor at any point over the graphic
item and then press Shift + P. A reference point gets placed there and that point will be
in the coordinate 0,0. Now move the cursor to any point of the graphic item to measure the
dimension.
Q12: I am not able to create a padstack for 5 layers but EDWin
provides creating the padstack for 32 layers. Is there any other method?
EDWin does not provide defining Padstack for 5 layers automatically. But you may proceed
in the following way. In Padstack Editor, select New Padstack using wizard and select the
tab New/ Edit. Type in the name and the required parameters. Click on show layers and
select the 5 layers which you intend to use and click Make Padstack. The picture clip
shown besides displays the padstack you created.
If necessary use the tools given and edit it manually.
Q13: How to create an elongated padstack?
In EDWin there is no special graphic tool provided to create an elongated padstack. So we
had adopted the following method to create an elongated padstack. Start a new padstack
from the scratch and place a line with larger Lsize. In normal view, this looks like a
simple line. Select View/True Size to get the elongated padstack view.
Note: While viewing padframes, switch on the true size to view the effect.
Q14: I want to replace the DIP24 package of a 74xx154 to the
SMD-package SOTxx. Is it possible to replace a package, or is it necessary to create a new
part with symbol and linked SOT package?
Yes, it is possible to replace the package without any problem provided the no. of pins is
not lesser than the previous one. This can be done in the following way:
Invoke Library editor, select the part whose package is to be changed and change the
package name in the package column and ENTER. Select File / Save Part.
Q15: How do I create a transformer with multiple secondaries
and transformers with a center tap secondary that will work in Mixed Mode simulator and in
EDSpice simulator?
In Mixed Mode simulation, you require a simulation primitive for each category of symbol
you wish to simulate; for example, as in your case, Transformer with single Secondary
winding, Transformer with 2 Secondary windings, Transformer with center tapped secondary
etc. This simulation primitive is attached with the relevant symbol for simulation.
Q16: Is it possible to create a package, which has through
holes, but no pads, with EDWin? (i.e. mounting holes). If so how?
While creating packages, choose the size of pad equal to the hole size of the padstack, so
there is no copper for the pad. Proceed as with any other package and you get a package
with a mounting hole, but no copper. If you want a mounting hole as such, just create a
package with a single padstack with properties as above.
Q17: I created a new component, Antycip.Part. I cannot find it
in library browser during search. Why? How can I have access to my own library?
If you have created your own library then first you have to add this particular library in
library search sequence in Library Browser module. To include this newly created part file
in the Search sequence, select the View/ Search Sequence menu from the Library Browser/
Library Explorer and check the corresponding, *.Part, *.Symbol, *.Package files that have
to be included in the Search list explicitly.
Q18: Creating a Symbol using the Library editor. I have some
pins in a part, which have no connections. Unless I define them in the Symbol, a mismatch
error occurs when I define a part. I would like the no connects to be invisible in the
Symbol and though the visibility column in a table in the library/edit Symbol/auto
generation process allow this......but it makes no difference. Do I misunderstand the
meaning of visibility here?
If so, is there any way I can generate a part with no connect pins, which does not show
them in the Symbol and avoids errors in the part generator?
You have really misunderstood the actual meaning. This option (visibility) may be used to
make pinout text for entries visible in the schematic diagram after packaging so that the
pin numbers of the entry points can be seen.
You do not have to create pins in Symbol for NC (No Connection) pins. If there are NC pins
in the part, just leave free the corresponding pin in the layout. The system automatically
takes it as a NC.
Note: Please make sure that all entries in the Symbol are assigned to one of the layout
pin for accurate part creation, and also do not assign more than one schematic entry to a
layout pin.
Q19: I have been struggling to figure out the difference
between the Library Browser and Library Explorer, what is their actual difference?
Library Browser:- This utility is used to browse a Part, Package, Symbol or Padstack
according some defined criteria. This can be used to find usage of Symbol, Package etc.
The user also have the provision to add types of Parts (View -> Register -> Part
Types). Working of this module is similar to WINDOWS Find. The Parts in the search output
list may be loaded to Schematic capture or Layout by "Send to"(from the right
click menu) or "Drag-Drop". This module supports Numeric Search (Alphabets in
the Part name ignored by the Search e.g. With numeric search enabled and searches for 7400
lists all SN7400, 74HC00, 7400D).
Library Explorer:- Working of this is similar to Windows Explorer conforming to EDA
standards. This supports Cut, Copy, Paste etc. Copying one library elements to other by
just drag - drop or Copy Paste, creating new library file etc. It can sort library
elements according to different criteria (there are 14 default criteria for Part, User can
add user-criteria.).
Q20: In Explorer, I have the option to Edit the part, but its
'grayed out’ (disabled). if I try to edit from the Browser, presumably because there
is no symbol associated with the part.
It should be noted that all Part files and associated Symbol and Package files must be
included in the Search Sequence for using or editing.
Q21: I cannot save to 74TTL.part, nor can I rename, cut, copy
or do any editing operations on them.
Library Files supplied along with EDWin as well as library elements (parts, symbols and
packages) stored in the currently loaded project (PROJECT LIBRARY) are SYSTEM LIBRARIES.
The System Libraries CANNOT be Deleted, Renamed, Cut etc. i.e. the user cannot alter the
System Libraries. You may however edit a System library Part/ Symbol/ Package but after
editing, it cannot be saved to any of the system library files. You may save it to a User
Library.
Q22: How can I edit Part/Symbol/Package in the project?
or
When I edit a part and want to update the changes to Project Library, the File à
“Update to Project Library” menu item is disabled.
You can edit Library objects residing in the Project library from Explorer or Drag Drop
into Library editor. The corresponding symbol and Package will be taken automatically. You
may save to USER Library if you want, Or you may cancel the Save operation. File à Update
to Project Library will update the changes in the Part in the Project Library and the
changes will be reflected in the Schematic /Layout Editors.
It is possible only to update to Project Library when a part in the Project library is
edited.
Q23: When I save the part (in the new library) and then try to
use it in the Schematic or Layout Editor, the changes seem to have disappeared and the
original part appears. As far as I can see, I am saving the part correctly and also
calling the correct part from the library browser / Explorer .
This is because you have not included the newly created library in the Search Sequence.
You may do so in the following way. EDWin 2000 à Library Explorer à View à Search
Sequence à activate the checkbox to the left of your custom library.
A brief note on the use of search sequence. You have three libraries say 74TTL.PART,
BASIC.PART and MyCustomLib.PART having the part 7400 and you prefer to load 7400 from
MyCustomLib.PART then you need to put MyCustomLib.PART higher than 74TTL.PART and
BASIC.PART in of the Search Sequence. The EDWin library has System Libraries supplied by
Visionics and Custom libraries created by you. In case you want to select library elements
only from your libraries just uncheck System libraries from the Search Sequence or put
your custom libraries higher up in the sequence using the arrow keys provided for the
same. If you have 100 Part libraries and you need 10 out of these for the particular
project then add these 10 to the Search Sequence, which will increase the Search speed and
efficiency.
Q24: I get the error message "Symbol/Package not
found"
This usually happens if you are using converted databases from EDWin 16 or an EDWin32.
Saving the Symbols and Packages to user libraries and subsequently adding them to the
Library Search Sequence will solve the problem. Also open Field Editor à Select the
library à Right click
Q25: How do I convert old package to new IPC and JEDEC standard
compliant names, egs from DIP14 to DIP14/300?
The Packages with OLD NAMES may be automatically converted using an option available in
Field Editor à Select Library à. Click in the right pane à Right click à Get EDWin
2000 Convention Package name. This option is not available in the Project Library.
EDWin 32 and EDWin XP/2000 libraries
Q26: Why do I need to use separate copies of libraries and
databases/projects for EDWin 32 and EDWin 2000 if all libraries are upward compatible?
Any attempt (even for browsing using Library Explorer or Browser) to access EDWin 32
libraries from EDWin 2000 environment causes permanent change of format of EDWin 32
libraries. EDWin 32 libraries and databases once used with EDWin 2000 cannot be used with
EDWin32. Therefore it is imperative to use separate copies of libraries and databases for
EDWin 32 and EDWin 2000.
Q27: How do I add a new manufacturer?
Library Browser à View à Register à Part Types à Select the Manufacturer Tab à
Right click on any of the entries à Add Top Level. Similarly new Type / Technology and
Package type can be added.
Q28: I need to create components with oval holes, I mean I need
not only OVAL padstack, the component pins are not cylindrical but are a small slabs so I
need a way to
define a slot in the center of the padstack. Can you give some hints or ideas about how to define this kind of holes in order to PCB manufacturing firm can understand my Gerber and
Drill files?
1. Create an Oval Padstack (Name:Oval) with the desired width (more than the width of slab
pin). This padstack should have a hole diameter just greater than the thickness of the
pin.
2. Create an Empty (Name:Empty) padstack with hole diameter equal to the hole diameter of
above padstack.
3. Create a New Package with the Oval Padstack as #1.
4. Then place and repeat the Empty padstack in both sides of the hole of above (Oval)
padstack. Adjust Grid and Snap properly in order to repeat and place the padstacks.
A similar Part with Slab Pin Package is attached. In that Oval padstack has width of
.1" and hole dia of .035" and Empty padstack has .035" hole dia. Go to
Package Editor and Place the Oval padstack. Draw a horizontal line through the centre of
the Padstack. Now repeat and place the empty padstack on both sides of Oval padstack entry
on the line. After placing necessary Empty padstacks delete the horizontal line. ->
Save Package -> Save Part.
|