importing schematic to eagle

[Anonymous]

Hello Sir,

 am working on conversion of components from altium tool to eagle.am unable to import schematic in eagle from altium. so i have to create component manually in the eagle.

Is ther any script which can make work easier.

Regards,

sushmitha

[Anonymous]

https://forums.autodesk.com/t5/eagle-forum/importing-files-from-altium-designer-to-eagle/td-p/682725...

[edwin.robledo · Accepted solution]

Hi sushmitha,

I hope you are doing well upon receiving this message.  There is an intricate ULP that makes to process of creating parts in EAGLE fairly easy. 

The ULP was mainly intended to import BSDL file, but it is capable to building parts as long as you input the component criteria.  

Autodesk is in the process of updating this system, but in the meantime your can use what we currently have.

From the EAGLE library editor, click on File/Import BSDL.  From their you can follow the prompts. I am attaching the help file that is available in PDF format.

FYI: User Language Programming (ULP) is a feature of EAGLE that allows the community to expand the capabilities of EAGLE by using a C-Like programming system. 

I hope this helps. 

Best Regards,

Ed

[Anonymous]

Thank you Sir, I would like to know  how can i get BSDL file from Altium , Allegro,and Mentor to import into Eagle 

[Anonymous]

sir,.is it possible to import .lia file into eagle?

[jorge_garcia]

Hi @Anonymous,

I hope you're having a good day. Unfortunately, at this point in time EAGLE can not import a .lia file from altium. The best we can import right now is PCAD ASCII files.

This is an area of EAGLE we are looking to improve. Please let me know if there's anything else I can do for you.

Best Regards,

Jorge Garcia

[Anonymous]

Hello Sir,

I imported P-CAD schematic file into eagle and everything is fine except the pin names are not imported.May i get the solution for this?

Regards,

Sushmitha

[rachaelATWH4]

---

@Anonymous wrote:

Hello Sir,

I imported P-CAD schematic file into eagle and everything is fine except the pin names are not imported.May i get the solution for this?

Regards,

Sushmitha

---

It looks to me like its drawn a polygon as the symbol body rather than lines to create a body outline which I suspect is obscuring the pin names. Try editing the library symbol and replacing the filled polygon with an outline drawn with wire tool.

Best Regards,

Rachael

[Anonymous]

Hello Sir,

Yes i have to add pin names for each and every pin which takes more time instead , pin names should appear at once while importing..how can this be done 

Regards,

Sushmitha

[rachaelATWH4]

---

@Anonymous wrote:

Hello Sir,

Yes i have to add pin names for each and every pin which takes more time instead , pin names should appear at once while importing..how can this be done 

Regards,

Sushmitha

---

Did you try what I suggested?

How are you adding the pin names? I suspect you are just adding text which is unrelated to the actual pin as a label.

Please try as I wrote above, i.e. remove the filled polygon which is likely obscuring the pin text and draw the symbol body manually with the wire tool to create an outline rather than a filled body then maybe it'll have the pin names.

I've never used the P-CAD importer as I have never needed to import any libraries from Altium but this would be my best guess for what is going on.

Best Regards,

Rachael

P.S. I am not a "Sir".....

[Anonymous]

Hello,

yes i removed the polygon and manually drew the wire but still i can't find the pin names.

the symbol is attached below.

[rachaelATWH4]

---

@Anonymous wrote:

Hello,

yes i removed the polygon and manually drew the wire but still i can't find the pin names.

the symbol is attached below.

---

Hello,

Issue the command:

CHA VIS BOTH

Then click on each of the pins. This should set the visibility of the pins to correctly show the both the pin names and numbers.

Also, in your image I can see you've drawn the body outline on the wrong layer, it looks like its likely drawn on the Names or Values layer when it should be on the Symbols layer hence it is grey rather than red.

Also, make sure you have the Names layer turned on in the schematics and library, in case its something as simple as the layer visibility is set to off.

Best Regards,

Rachael

[Anonymous]

hello,

yes the method u said is manually ticking 'visible -both option'.this can be done for less number of pins but when there is more number of pins this method is tedious.

so what i have done is imported P-CAD V16  schematic netlist and made few changes in netlist to display pin names globally.

but the changes ,made in netlist isn't working.

Regards,

Sushmitha

[rachaelATWH4]

---

@Anonymous wrote:

yes the method u said is manually ticking 'visible -both option'.this can be done for less number of pins but when there is more number of pins this method is tedious.

---

Not quite... My suggestion above is issuing the given command from the EAGLE command line within the symbol editor. Then you can perform the change operation on a group of pins.

So the workflow is:

1. Ctrl+A to group the entire symbol (which will include all the pins)

2. CHA VIS BOTH to start the change operation

3. Ctrl+Right Click to perform the operation on the entire group.

It doesn't matter whether your symbol has 2 pins or 2000 pins, it's the same operations above performed and it'll only take a few seconds per symbol to change it.

Best Regards,

Rachael

[Anonymous]

Hello,

Thank you so much. This solution was very helpful to me.Thank you again..:)

Regards,

Sushmitha

[Anonymous]

Hello,

same as schematic the command you gave to enable pin names is there any command to print all the solder mask and paste-layer into the footprint imported?

Regards 

Sushmitha

[Anonymous]

i meant mainly on copper shapes are not been imported into eagle is there any command..to get it?

[rachaelATWH4]

---

@Anonymous wrote:

i meant mainly on copper shapes are not been imported into eagle is there any command..to get it?

---

Do you mean only on pads which are a custom shape or on any pad, even standard ones? If you mean any pad, are they not set or are they just not shown? Make sure you have tStop and tCream turned on and if they are not see if they are actually there when the layers are turned on.

If you need to enable stop mask and paste mask generation then in the library editor, in the package do the following:

1. Ctrl+A to group the entire symbol (which will include all the pins)

2. CHA CRE ON to start the change operation

3. Ctrl+Right Click to perform the operation on the entire group.

4. CHA STO ON to start the change operation

5. Ctrl+Right Click to perform the operation on the entire group.

IMPORTANT NOTES:

1. If you have pad shapes in your imported footprints which are created with polygons and there are not corresponding polygons on the tStop and tCream layers to specify these from the import process, then you'll have to use the datasheet recommendations to create similar polygons on these layers to give the appropriate shapes on the tStop and tCream layers.

2. Some parts are specifically designed to NOT use the auto generated tStop and tCream because they are too fine pitch for this to work correctly. In this case you'll need to create them manually, ensuring you follow the recommendations in the manufacturers datasheet.

Best Regards,

Rachael

[Anonymous]

HELLO

I followed the same procedure but it isn't working. i have attached two images where one is the image from altium and one is image imported to eagle with missing copper pads.

Regards

Sushmitha 

[rachaelATWH4]

---

@Anonymous wrote:

HELLO

I followed the same procedure but it isn't working. i have attached two images where one is the image from altium and one is image imported to eagle with missing copper pads.

Regards

Sushmitha 

---

Hello,

This is what I was referring to in my IMPORTANT NOTES section. Both the points there are relevant here. The auto generated tStop and tCream are not good on this part so should be turned off and they should be created by hand.

In addition it seems that the importer is not creating anything which includes custom pad shapes so you're going to have to draw all these yourself I'm afraid. You'll need to place small regular SMD pads in the middle and then draw the remainder of the pads ensuring they encompass the entire SMD pad. If you need to learn how to do this then I wrote a library creation tutorial which will explain how to do this here: EAGLE Tutorial: Library Part Creation Part 4 - Advanced Packages and Package Variants

Best Regards,

Rachael