Mentor Library questions

[john5888]

mentor questions

Hi,
I am trying to change from P*otel to Mentor
I found that Mentor 2002 seems not including the library as many as
P*otel or orcad, it just have a few symbols and footprints,
my question is, does it all need to created by myself?
If so, the job will be very hard.

Thanks

 

[Kevin]

mentor different pins same name

u must creat it's and manager it's with lib manager by uself

 

[CADPCB]

tutorial dxdesigner symbol

Hi,
I am trying to change from P*otel to Mentor
I found that Mentor 2002 seems not including the library as many as
P*otel or orcad, it just have a few symbols and footprints,
my question is, does it all need to created by myself?
If so, the job will be very hard.

Thanks

****************************************
well difference in price is telling you difference in tool. Is it worth changing ??

 

[binu G]

update lmc dxdesigner create part

it is a tedious job for creating a library for each components better the provider should provide the common lib

 

[sigint]

mentor library manager

M/E/N/T/O/R supplies nothing with it's software - everything is additional - the basic program costs this much - if you want to generate gerbers it costs more, (really, I'm not kidding), if you want to export HPGL it costs more, it goes on forever - there are probably libraries available as an add-on.

SiGiNT

 

[lesuisse]

mentor library services import symbols ascii

Hello,

I disagree about the statement on WG2002.
The VBCORE library is substantial nevertheless you need to make your own based on that VBCORE.
With a little practice it is extremely easy and you can do many parts in one day.
Additionally, you can have for each project a local library that will contain only the parts needed for the project.

If you need any help in creating parts, just post me and I'll do my best to help.

Lesuisse

 

[sigint]

mentor expedition without central library

I agree that creating parts and schematic symbols is not all that difficult, but, I've run in to more than a few designers that seem to have difficulty with doing that, maybe it doesn't hold their attention, modifying existing parts is faster and more productive. If you compare what comes standard with most other packages - M/E/N/T/O/R's high-end products give you next to nothing at the "basic" price level - with W/G/2/0/0/2 you will notice that gerber generation was broken off into a separate "CAM" package that will require a separate license - in the past this function was always included in the layout package. My comment was not directed at the software at all, just about how it is being sold.

SiGiNT

 

[Santa]

mentor library cell

Some update on the WG library topic...

With WG2004, the situation is worse than ever. You get no library
with it. So you have to build your library from scratch.

On the opposite to what was said, building components that follow all the
rules and philosophy of WG is not so simple. There are many hidden traps
that, for a beginner, will show up only much later when your library is already well filled
and that could require that, at best, you need to update all your components,
cells, symbols or padstacks.

So my opinion is that:
- the basic library that was given with WG2002 was insufficient. At least
all common cells should have been defined.
- It is even worse now and a shame from a big company like Mentor for
such an expensive package.

 

[Uky]

mentor library

Indeed MG does not supply a free library, but I can understand why: There are not two company structures that resembles one another, not to library definitions that resembles one another and MG gives you a wealth of options how to create your company library. You must realize that the WG in WG200x stands for "Work Group". This software is not intended as a personal productivity tool, it is intended for small to medium sized companies that realizes that they need a standardized integrated PCB productivity tool where the library does not consist of footprints and schematic symbols, but on _parts_ that have undergone your organizations qualification procedure.

Once you get the hang of how to design your busines library, you will find that creating and maintaining your own library is a smooth and quite simple procedure. You will also realize that you are better off without having a large library of parts that does not meet your requirements or that they all have to be modified.

Of all PCB CAD systems that I have used, I have NEVER found the included (if any) libraries to be useful. I have had to sit down and create them from the bottom up, starting with the components for my first project, and added parts as I went along. There is no need to create an entire logic family or the complete E96 series of resistors just for one small PCB.

The number of footprints and schematic symbols is relatively small compared to the number of components (parts). It is in the parts manager function that everything is tied together and it is in this function that WG really excells. Once one part i.e. resistor is created, it is a matter of seconds to copy the part and change [resistance] values.

I can see that a user who encounters this software for the first time panics by the complexity of it and the lack of manuals describing it in a simple and basic way. The documentation describes it thoroghly, but does not give any recommendations on how to configure it.

And Yes - I agree: Gerber output should be included in the base product and not as an "Add-on"

WG may not be the ultimate product for someone who just wants to design smaller boards, or who uses PCB design software infrequently. The software is expenceive, and anyone who uses it soon realizes that a maintenance agreement is a must. Think twice before you start to use it.

 

[Santa]

mentor library manager manual

The problem is not so much receiving a free all-purpose library. There is
not such a thing that will make anybody happy and, like everyone, I had
to change partition organization, add new properties, etc...

However, some kind of clean library is very much needed by the beginner as an
example to learn the tricks of WG and, as said, where things are much more
standard like cell patterns, it would be a lot of time saved for the user.

I admit however that some issues with design rules of the padstacks linked
to the production process could come in the way of a standard cell/pads
library.

The fact that wg means workgroup is probably not linked to the size of
the target company in the mind of Mentor but to the fact that the engineers may
cooperate on building new objects (pcbs, libraries, etc...) like a team.
The high price tag of the suite and the last features going further in this
direction like teamPCB or IODesigner demonstrate this.

 

[smithchart]

iodesigner export

Hi, All:

I just started to use wG a few days ago with the help from its tutorial. It's really frustrating that I cannot find its standard library for general purpose usage (Maybe I didn't find where it is).
In addition, when I try to generate the symbol of a 244CBGA package, I used the symbol wizard, I found that the Wizard is very weird in the sense that: it has the capability of exporting symbol characteristics such as name, label etc. as an ASCII file which can be edited using Excel conveniently. However, it can not be reimported into the wizard, nor can it be copy/paste as blocks into the input table of the wizard! Another thing and maybe a bug is: wizard cannot support those pins that share the same label such as Vss/Vdd etc. Really frustrating!
Can any expert here give me some tips on using it as a beginner?

Thanks and Best Regards,

 

[Santa]

questions for a mentor

Hi, search for a file having the .lmc file extension but normally it is
not provided starting with version 2004.

As for the problems not having a sample library to show you how to do things,
I see you understand my point...

For the rest, I don't understand why you are mixing symbols and cell (packages)
topics. In WG, these objects are very much different and linked at the
device level in the library, not sooner.

As for exporting/importing, you may do so to or from an ascii file although
I detected a bug in the library services that doesn't show any part(s) to import
from ASCII until you play a bit with the buttons of the dialog box. I know this
in the ExpPCB library services but it could also be true for the Library Manager
if they share some code.

As for having two pins with the same name, it is not allowed. This fact shouldn't
be much of a concern. Call them VCC1, VCC2, etc and make them swappable.

 

[Uky]

mentor lmc library sample

Smthchart, Starting as a beginner with PCB layout and then choosing WG.... Respect! You can find basic footprint (cell) libraries on the internet free for downloading. on several sites. Just use your favourite search engine. You will then have to create the schematic symbols and the parts in the Library Manager. Once you get over this treshold, you will find that WG is a well designed system and easy to use, although with a few flaws, amongst them that it may crasch and you will have to rebuild the library index, unlock cell partitions and so on.

Frequent backups of your library is strongly recommended!

As Santa writes, you can not have two pins using the same name, but there is a circumvention: If you have say four pins "GND", name them GND1...GND4. Then make the names invisible, and add arbitrary text "GND" to all the ground pins. I do not like this myself, but it makes your symbols look nicer.

 

[smithchart]

powerpcb invisible pin name

Hi, Santa and Uky:

Thank you two for the explanations. I partially solved the library reuse problems and now with more understandings of the system, I think it's better to create my own library from scratch.

The package I am using is MentorGraphic SDD2004, the design flow I am going to use is: DxDesigner for schematic, Library manager for parts generation(including symbol creation, padstack and cell generation), and Expedition for PCB layout. Since I am new to PCB design without any trainning, I found the online help system/tutorial is rather insufficient and poorly orgnized. For example, the DxDesigner tutorial is supposed to talking about DxD-->Expedition design flow, however, what the tutorial did is simply introduced the Dxdesigner and then divert to PowerPCB flow which is not part of the SDD package.

Just to share with you two the way I reused the libraries:
1. Using library manager to create you own central library
2. Copy all the cells and padstack files from WG2002\vbcore\central library
3. Import symbols from eProduct Designer Libraries provided by MentorGraphic
For the above flow, you can see that we cannot reuse the symbols from WG2002 central library(don't know why).

Well, I am now trying to generate a 244ball BGA package cell and encountered a probelm: I used 16 x 16 matrix to generate 256balls and late delete the redundant balls. After I finished all of these steps, I found the cell editor does not allow me to save the file with a pop up error of: the cell cannot be saved because 12pins are not placed. I am trying to find the solution by searching the online help now and also hope some of the experts here can help me. (maybe I can also leave the extra balls there but I am afraid that will get into trouble when I proceed to the stage to associate the cell with my 244 pin symbols to create a part).

By the way, is there any standard talking about how to generate PCB land patterns for different kinds of ICs such as BGA, VQFN etc?

Thanks!

 

[smithchart]

mentor expedition central library

Hi,

I've solved the cell generation problem raised in the last post, there are two methods:

Method1:
a. Define the exact pin numbers you want at the very beginning, say 244.
b. Define the new pins to make the layout an array: another 12 pins to make the layout 16x16 array
c. After pin place, delete the extra pins and save

Method2:
a. Define the array directly:16x16 and save
b. Use cell editor to change the property: pin number changed from 256 to 244 (this is done in the library manager and from the new cell generation dialog )and then in the GUI to delete the extra pins before saving it.

 

[Uky]

dxdesigner local symbol partition file

The fact that the user can not save an incomplete cell during creation is an annoyance with Mentor (Expedition) Library Manager. It has been a long standing open issue.

ANY user would want to make partial saves during cell editing, and this basic functionality isn't there >> sigh <<

I had one case where I was creating a 400+ pin BGA with irregular pattern. In the middle of my work there was a system hickup....

Now that was v e r y amusing...

 

[Uky]

• wg2002 central library

The fact that the user can not save an incomplete cell during creation is an annoyance with Mentor (Expedition) Library Manager. It has been a long standing open issue.

ANY user would want to make partial saves during cell editing, and this basic functionality isn't there >> sigh <<

I had one case where I was creating a 400+ pin BGA with irregular pattern. In the middle of my work there was a system hickup....

Now that was v e r y amusing...