Author Message
 Post subject: Librarys, Components, Pattern. I cant get a handle on this..
PostPosted: 20 Aug 2017, 18:10 
Offline

Joined: 19 Aug 2017, 10:22
Posts: 3
Frankly I am a bit frustrated and overwhelmed. I am a hobbyist not an electronics engineer. I have used ExpressPCB to make Schematics and PCB designs in the past, but I wanted to use a program that was not proprietary to one PCB manufacturer. After reading many reviews of software, I decided Dip Trace was the way to go. I have spent hours doing the tutorial several times and looking thru this forum and watching YouTube vids. I have referred to several posts offering help with setting up and managing libraries and I still just can't seem to get my head around how to use this software. In the Express software, I start by selecting "Place Component" scroll down to 'Connector - wire' and click to place a "lollipop" representing a wire connected to my circuit. When making a PCB, I select "Place Pad" and select an appropriate "standard" pad to place on the board. I could select a component, modify it to match my desired pattern, save it to my user library, and continue my PCB design...
Now, even after all this time trying to learn how to use Dip Trace, I can't even get started on my Schematic. I keep searching thru huge libraries to find a suitable "wire connector" for my drawing. I can't to attach it to a pad dimension for my PCB. I try get the software to let me pick a pattern, modify it and save it to the User Library I set up with the Library Management guide on this forum. I expected to find a NEW COMPONENT button to start designing a part from scratch. In the Component Editor. If I go to COMPONENTS, PINS, PINSHAPE-D50 I find an appropriate symbol for my drawing, but of course it has no component or pad associated with it. I use PATTERN button and similarly select an appropriate pad for the PCB, but I can't seem to get to the correct list of PADS where I can choose or edit the dimensions so I select Round - Round and Ok. Now I have to go back to "Libraries" and find my User Component Library. I still can't figure out how to save it as a new component. I have also spent several hours trying to choose an existing component, i.e. IRLML2803, change it to IRLML6346 and save it to my User Library. There is obviously something I am missing about how Dip Trace handles all this, but it's not sinking in. Can anyone offer a resource that might help me understand the basics of this? Somehow it eludes me.


Top
 Profile  
 
 Post subject: Re: Librarys, Components, Pattern. I cant get a handle on th
PostPosted: 21 Aug 2017, 14:08 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 940
Reading your post, it looks like you have already seen the library setup thread located here - http://www.diptrace.com/forum/viewtopic.php?f=5&t=10937. The explanation below assumes that you are a beginner at this (obviously, you are not), but humor me by reading it as a "first-timer" might...

PATTERN
A pattern (footprint) is the physical representation of a device (copper pads, silkscreen, etc.) and is what appears in the PCB layout. Patterns are typically designed in the Pattern Editor and attaching a 3D model to the pattern is optional.

COMPONENT
A component is a combination of a pattern (copper pads, silkscreen, etc.) and an electrical representation of a device (drawing symbols with electrical pins) that is used in both the schematic (drawing symbols with electrical pins) and the PCB layout (copper pads, silkscreen, etc.). Before a component can be used in the PCB layout, a pattern needs to be attached to it using the Component Editor to assign connections between pattern pads and component pins. If a component has no attached pattern, there will be no associated pattern showing up in the PCB layout. (See the section titled "Attaching a pattern to a component" below.)

SCHEMATIC
The schematic contains all of the desired components (drawing symbols with electrical pins) for your circuit design with connections (wires) between their pins. Common/shared connections are referred to as Nets and the collection of Nets used in a design is what is referred to as a Netlist. The Netlist is responsible for maintaining proper connectivity between all of the component pins/pads in both the schematic and the PCB. The Netlist also allows for automated electrical checks to be performed to help catch any possible wiring (schematic) and routing (PCB) errors.

PCB
Once the schematic is complete and has been saved, you can bring the circuit from the schematic into the PCB layout using one of two methods. The first method involves pushing it into a new PCB using the Convert to PCB tool in the Schematic Editor. The second method involves pulling any schematic changes into an existing PCB using the Renew Layout from Schematic tool (choose the By Components option) in the PCB Layout editor.

LIBRARY
A DipTrace library is a single file that contains multiple parts. For example, a pattern library file can contain multiple patterns and a component library file can contain multiple components.

LIBRARY GROUP
A library group is a folder that exists only within the DipTrace library manager and is used to group together and organize multiple library files of the same type for convenient access by the user. The five main DipTrace library groups are named "Components", "Patterns", "User Components", "User Patterns" and "Project Libraries". The "Patterns" and "Components" groups contain links (names) pointing to the standard libraries that come with DipTrace and cannot be changed. The "User Patterns" group contains links (names) pointing to custom pattern libraries created by the user. The "User Components" group contains links (names) pointing to custom component libraries created by the user. The "Project Libraries" group consists of links (names) pointing to libraries containing project patterns and components saved by the user. Other library groups can be created if needed.

-------------------------------------------------------------------------

Pattern Editor - creating a new custom pattern
1) In the Select Pattern window on the left side of the Pattern Editor, click on the Current Library Group selection box and choose the User Patterns group in the fly-out menu.
2) Select the desired custom pattern library in the library list just below the Current Library Group selection box.
3) Click on the Pattern Tools box just below the Library Tools box and choose Insert New Pattern to "[library name]" Library in the fly-out menu.
4) A new blank pattern named "Untitled" should now be displayed above the previously-highlighted pattern in the patterns list (below the Pattern Tools box). If the newly-inserted blank pattern is not highlighted in the patterns list, click on its name to select it. The Design Area should now be blank. Note: The Design Area displays the pattern that is selected/highlighted in the patterns list.
5) In the Pattern Properties dialog window, enter the desired pattern name in the Name: box and enter the desired reference designator prefix in the RefDes: box.
6) To set up the default pad size and shape, click on the [Pad Properties...] button. You can also select a pattern style using the Style: drop-down list.
7) After your pad layout is finished, add any necessary silkscreen and/or other objects.
8) Resave the custom library (Ctrl + S).

-------------------------------------------------------------------------

Pattern Editor - creating a new custom pattern by modifying a standard pattern
To modify a standard DipTrace pattern, copy it to a custom pattern library, modify it there, resave the custom pattern library and then use the modified custom pattern. To create the modified custom pattern...
1) In the Select Pattern window on the left side of the Pattern Editor, click on the Current Library Group selection box and choose the User Patterns group in the fly-out menu.
2) Select the desired custom pattern library in the library list just below the Current Library Group selection box.
3) Click on the Pattern Tools box just below the Library Tools box and choose Insert Patterns from Another Library... in the fly-out menu.
4) In the Insert Patterns dialog window under "Libraries", select Patterns in the drop-down list, select/highlight the standard DipTrace library that contains the desired pattern, select/highlight the desired pattern in the list under "Patterns" and click on the [Insert] button.
5) The inserted pattern should now be displayed in the Design Area and selected/highlighted in the patterns list in the Select Pattern window. Note: The Design Area displays the pattern that is selected/highlighted in the patterns list.
6) Make the necessary changes to the pattern.
7) Resave the custom library (Ctrl + S).

-------------------------------------------------------------------------

Component Editor - creating a new custom component
1) In the Select Component window on the left side of the Component Editor, click on the Current Library Group selection box and choose the User Components group in the fly-out menu.
2) Select the desired custom component library in the library list just below the Current Library Group selection box.
3) Click on the Component Tools box just below the Library Tools box and choose Insert New Component to "[library name]" Library in the fly-out menu.
4) A new blank component named "Untitled" should now be displayed above the previously-highlighted component in the components list (below the Component Tools box). If the newly-inserted blank component is not highlighted in the components list, click on its name to select it. The Design Area should now be blank. Note: The Design Area displays the component that is selected/highlighted in the components list.
5) In the Component Properties dialog window, enter the desired component name in the Name: box and enter the desired reference designator prefix in the RefDes: box.
6) Create the desired electrical symbol using the drawing tools at the top of the screen.
7) Add the needed electrical pins, arrange them as required ([Space] bar rotates them), click on the [Pin Manager...] button in the Component Properties dialog window, define each pin using the Name:, Number:, Electric: and Length: entry boxes and select OK.
8) Attach the desired pattern. (See the section titled "Attaching a pattern to a component" below.)
9) Resave the custom library (Ctrl + S).

-------------------------------------------------------------------------

Component Editor - creating a new custom component by modifying a standard component
To modify a standard DipTrace component, copy it to a custom component library, modify it there, resave the custom component library and then use the modified custom component. To create the modified custom component...
1) In the Select Component window on the left side of the Component Editor, click on the Current Library Group selection box and choose the User Components group in the fly-out menu.
2) Select the desired custom component library in the library list just below the Current Library Group selection box.
3) Click on the Component Tools box just below the Library Tools box and choose Insert Components from Another Library... in the fly-out menu.
4) In the Insert Components dialog window under "Libraries", select Components in the drop-down list, select/highlight the standard DipTrace library that contains the desired component, select/highlight the desired component in the list under "Components" and click on the [Insert] button.
5) The inserted component should now be displayed in the Design Area and selected/highlighted in the components list in the Select Pattern window. Note: The Design Area displays the component that is selected/highlighted in the components list.
6) Make the necessary changes to the component.
7) If necessary, attach the desired pattern. (See the section titled "Attaching a pattern to a component" below.)
8) Resave the custom library (Ctrl + S).

-------------------------------------------------------------------------

Attaching a pattern to a component
1) Launch the Component Editor and select the User Components library group.
2) Select/highlight the component library that contains the component.
3) Select the component in the components list. The component should now be displayed in the Design Area. Note: The Design Area displays the component that is selected/highlighted in the components list.
4) In the Component Properties dialog box, click on the [Pattern...] button to bring up the Attached Pattern dialog window. In the Attached Pattern dialog window, the component should already be selected/highlighted in the list on the left side. If not, click on it to select/highlight it.
5) On the right side of the Attached Pattern dialog window, go to the Pattern Libraries drop-down list and select User Patterns.
6) In the Pattern Libraries list select the name of the pattern library where the desired pattern resides.
7) Attach the pattern to the component by finding the pattern in the Patterns list and clicking once on its name.
8) The component's pins should automatically be connected to the pattern's pads. If they aren't, you can either drag wires between them or use the Pin to Pad Table.
9) Click on OK. Sometimes DipTrace does not detect the changes that have been made so as a precaution click once more on the already-selected/highlighted component name in the Component Editor window before saving.
10) Resave the component library (Ctrl + S).

-------------------------------------------------------------------------

Creating a new pattern library
1) In the Select Pattern window on the left side of the Pattern Editor, click on the Current Library Group selection box and choose the User Patterns group in the fly-out menu.
2) Click on the Library Tools box just below the library list and choose New Library... in the fly-out menu.
3) In the Create New Library dialog window, enter a new library name in the Name: box (this is the name that will appear in the library list), enter a short description in the Hint: box (this is the pop-up message that will appear when mousing-over the library name), make sure the User Patterns library group is selected/highlighted and click on OK. The new library name should now appear selected/highlighted at the bottom of the library list.
4) Initiate a save of the new library (Ctrl + S).
5) In the Save As dialog window navigate to the folder where your custom pattern libraries are kept, enter the desired library name in the File name: box and click on the [Save] button.
6) In the Main Menu click on Library and select Library Setup... in the drop-down menu.
7) In the Library Setup dialog window select/highlight User Patterns in the Groups list, find and select/highlight the new library in the Group Libraries list, use the arrow buttons to move the new library to the desired location in the list and click on OK. You should now find the new library name at the same position on the library list located inside the Select Pattern window on the left side of the Pattern Editor.

-------------------------------------------------------------------------

Creating a new component library
1) In the Select Component window on the left side of the Component Editor, click on the Current Library Group selection box and choose the User Components group in the fly-out menu.
2) Click on the Library Tools box just below the library list and choose New Library... in the fly-out menu.
3) In the Create New Library dialog window, enter a new library name in the Name: box (this is the name that will appear in the library list), enter a short description in the Hint: box (this is the pop-up message that will appear when mousing-over the library name), make sure the User Components library group is selected/highlighted and click on OK. The new library name should now appear selected/highlighted at the bottom of the library list.
4) Initiate a save of the new library (Ctrl + S).
5) In the Save As dialog window navigate to the folder where your custom component libraries are kept, enter the desired library name in the File name: box and click on the [Save] button.
6) In the Main Menu click on Library and select Library Setup... in the drop-down menu.
7) In the Library Setup dialog window select/highlight User Components in the Groups list, find and select/highlight the new library in the Group Libraries list, use the arrow buttons to move the new library to the desired location in the list and click on OK. You should now find the new library name at the same position on the library list located inside the Select Pattern window on the left side of the Component Editor.

-------------------------------------------------------------------------

Removing a library from the User Patterns library group
1) In the Select Pattern window on the left side of the Pattern Editor, click on the Current Library Group selection box and choose the User Patterns group in the fly-out menu.
2) In the Main Menu click on Library and select Library Setup... in the drop-down menu.
3) In the Library Setup dialog window select/highlight User Patterns in the Groups list, in the Group Libraries list find and select/highlight the library to be removed, click on the [Delete] button and choose OK. This does not delete the library file. It merely removes the library name from the group's library list located on the left side of the Pattern Editor.

-------------------------------------------------------------------------

Removing a library from the User Components library group
1) In the Select Component window on the left side of the Component Editor, click on the Current Library Group selection box and choose the User Components group in the fly-out menu.
2) In the Main Menu click on Library and select Library Setup... in the drop-down menu.
3) In the Library Setup dialog window select/highlight User Components in the Groups list, in the Group Libraries list find and select/highlight the library to be removed, click on the [Delete] button and choose OK. This does not delete the library file. It merely removes the library name from the group's library list located on the left side of the Component Editor.

-------------------------------------------------------------------------

Deleting a pattern from a custom pattern library
1) In the Select Pattern window on the left side of the Pattern Editor, click on the Current Library Group selection box and choose the User Patterns group in the fly-out menu.
2) Select the desired custom pattern library in the library list just below the Current Library Group selection box.
3) Find and select/highlight the pattern to be deleted in the patterns list just below the Pattern Tools selection box.
4) Click on the Pattern Tools box and choose Delete Patterns in the fly-out menu.
5) In the Confirm dialog window, click on the [Yes] button. Now the selected/highlighted pattern should no longer be listed.
6) Resave the custom pattern library (Ctrl + S).

-------------------------------------------------------------------------

Deleting a component from a custom component library
1) In the Select Component window on the left side of the Component Editor, click on the Current Library Group selection box and choose the User Components group in the fly-out menu.
2) Select the desired custom component library in the library list just below the Current Library Group selection box.
3) Find and select/highlight the component to be deleted in the components list just below the Component Tools selection box.
4) Click on the Component Tools box and choose Delete Components in the fly-out menu.
5) In the Confirm dialog window, click on the [Yes] button. Now the selected/highlighted component should no longer be listed.
6) Resave the custom component library (Ctrl + S).

-------------------------------------------------------------------------

Deleting a pattern library file completely
1) Remove the desired pattern library from the Users Patterns library group. (Refer to the section titled "Removing a library from the User Patterns library group" above.)
2) Locate the folder where custom pattern libraries are stored and delete the desired pattern library file (*.lib).

-------------------------------------------------------------------------

Deleting a component library file completely
1) Remove the desired component library from the Users Components library group. (Refer to the section titled "Removing a library from the User Components library group" above.)
2) Locate the folder where custom component libraries are stored and delete the desired component library file (*.eli).

-------------------------------------------------------------------------

Once your component has been completed and the library in which it resides saved, it can be used in the schematic and then brought into the PCB using one of the methods described in the PCB topic at the top of this book. If you haven't yet read it, there is a reasonably thorough explanation of how DipTrace handles forward propagation here - http://www.diptrace.com/forum/viewtopic.php?f=3&t=11277. Let me know if you need any more information or if you spot any errors in my instructions.

_________________
Tom


Last edited by Tomg on 23 Aug 2017, 09:27, edited 9 times in total.

Top
 Profile  
 
 Post subject: Re: Librarys, Components, Pattern. I cant get a handle on th
PostPosted: 21 Aug 2017, 21:43 
Offline

Joined: 19 Aug 2017, 10:22
Posts: 3
Tom, THANKS so much for your very detailed and helpful reply! After following your instructions I was able to successfully create a new pattern and component (a single hole with a silkscreen circle). I am still a bit confused by the whole "Libraries" thing but I am beginning to understand how to manipulate some of it. I think my problem is in understanding how the libraries are treated as files and where they are. I never fully understood how a DATABASE works either. I am used to each component having a file in a folder that could be copied, opened, edited, and "Save As"ed from one screen. I am beginning to understand the meanings of "Add New Component to..", "Insert New Component to.." and Insert Component from.." and the idea that saving a component means saving the whole new library... Still a bit fuzzy, but I'm getting there. I keep ending up with multiple libraries within my User Library that give me errors like "This file is blocked by (Computername), would you like to make a COPY in (Someother Library)?" and an extra library full of MyComponent COPY and MyComponent COPY COPY, and trying to delete them, but that may be another issue? I think if I keep plugging at it one day I will wake up with an epiphany and it will all make sense.
Thanks again for your help!


Top
 Profile  
 
 Post subject: Re: Librarys, Components, Pattern. I cant get a handle on th
PostPosted: 22 Aug 2017, 00:02 
Offline

Joined: 18 Dec 2015, 15:35
Posts: 161
Something I wasn't aware of that Tomg didn't mention is Library management, without understanding how to build libraries your parts have no home.

First decide what it is your building, project with one board or many? If it is one PCB you could save your libraries with other projects under a common Group name, if your project has many boards then you might need a Group for that project by itself. If you need a Group you'll need a directory for that Groups libraries, you can share a directory with other Groups BUT cleanup, backup, sharing and exporting gets ugly. I learned that DipTrace is really happy with C:\Users\Kevin\Documents\DipTrace and in that location it builds folder called My Libraries as the default location for user libraries. The built in DipTrace Libraries are all located at C:\Program Files\DipTrace\Lib with *.eli Component and *.lib Pattern. You can't move them or edit them. If you need to edit a pattern or component you MUST copy the part to your user/project library and edit it there. In my setup I have C:\diptrace\project and under project each project has ProjectName\library - pdf - 3d
EXAMPLE:
Image
Using Library Setup I add a Group for a new Project AFTER I have created a folder for the new project Alpha as in C:\diptrace\project\alpha add library + 3d + pdf folders in the alpha folder. Image
Once the folders are built add the Group
Image
Add a new library in the Group Alpha by using the Library Tools/New Library I'm calling it MainPCB and I'm putting it in the Project Alpha Group with a Hint of 'Main board'
Image
When you click the Save ICON (floppy top left) it will ask for a file name, this is because DipTrace allows you to name a library and name it's container (file) something different.
Image
In rehash: Group contains libraries either pattern or component. Libraries have locations and once there should not be moved, when you edit a part with pattern editor or component editor and try to update the schematic or PCB they know where the library was, it had better still be there. And this is why you move your libraries to C:\diptrace, if you share a project or try to troubleshoot a project getting everything to someone is a pain.
Next start Pattern Editor, Top Left select Library Group Project Alpha, Library Tools/New Library - fill in the fields
Image
Again click the disk ICON to save and enter the file name mainpcb - Open Library/Library Setup and you should see 2 MainPCB under Group Libraries, one is the pattern library and the other is the component library, in the Library Setup you can see both but in pattern editor or component editor you will see one.
For a portable project you should look at putting all the PDF and 3D files into the project directory.
Just trying to write about library management is confusing but it works and really is a flexible system.


Top
 Profile  
 
 Post subject: Re: Librarys, Components, Pattern. I cant get a handle on th
PostPosted: 22 Aug 2017, 07:56 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 940
I have added definitions for "Library" and "Library Group" to my original post above. I'll continue to update the original post if I can think of more ways to further clarify the DipTrace library system.

Added instructions for creating new pattern and component libraries.

Added instructions for removing libraries from their respective library groups.

Added instructions for deleting patterns/components from their respective libraries.

Added instructions for completely deleting a pattern/component library file.

Khordan wrote:
"...I keep ending up with multiple libraries within my User Library that give me errors like "This file is blocked by..."
When you see an error message telling you that an action you want to take on a library is "blocked", it usually means that the same library is already selected/highlighted in another open editor. If that is the case, go to the other open editor and select/highlight a different library to unblock the actions you're attempting in the first editor.

_________________
Tom


Last edited by Tomg on 23 Aug 2017, 09:28, edited 1 time in total.

Top
 Profile  
 
 Post subject: Re: Librarys, Components, Pattern. I cant get a handle on th
PostPosted: 22 Aug 2017, 16:53 
Offline

Joined: 18 Dec 2015, 15:35
Posts: 161
Tomg wrote:
Khordan wrote:
"...I keep ending up with multiple libraries within my User Library that give me errors like "This file is blocked by..."
When you see an error message telling you that an action you want to take on a library is "blocked", it usually means that the same library is already selected/highlighted in another open editor. If that is the case, go to the other open editor and select/highlight a different library to unblock the actions you're attempting in the first editor.


Or you Double Clicked on one of the editors in the DipTrace Launcher and the first click editor took possession of the library, the second click editor is the one you see with an error. Moving your library files nor flagging them READ/WRITE Shared will fix this, renaming the library works but you end up with a lot of libraries!
Don't use the DipTrace Launcher or learn how to single click....


Top
 Profile  
 
 Post subject: Re: Librarys, Components, Pattern. I cant get a handle on th
PostPosted: 23 Aug 2017, 20:30 
Offline

Joined: 19 Aug 2017, 10:22
Posts: 3
Great information! THANKS Tomg for the added information and instructions on Libraries, and Thanks KevinA for taking time to post the screenshots to clarify your examples of library management. You have both helped to enlighten me! I have a much better understanding of the concept of the libraries and how they remain linked to the Schematic Capture and PCB Layout. I believe the source of my frustration was treating Symbols and Patterns as if they existed independently. For example, A word document can be opened, then edited, then saved, or saved as a new document. In Dip Trace, I needed to realize that the Pattern Editor is the "Pattern Library Editor". That is, the Component or Pattern in the Design Area is IN the library it is pointed to, not an independent copy of it. Thinking of it this way I can see why I was having so much trouble. It also makes it clear why a library can't be open in two modules at once, although this possibly could have been hinted in the error message. It will be a few days until I can play with it more, but I am confident it will be much easier for me now.


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 7 posts ] 

All times are UTC - 5 hours [ DST ]


Who is online

Users browsing this forum: No registered users and 1 guest


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group