Can't import LTSpice schematic into Eagle project

Question

Hello,

I have no experience with Eagle and very very limited experience with LTSpice (a couple of months). In fact I have little experience with electronics hardware (I am a retired software engineer). I installed LTSpice IV on Windows 7 running on Parallels on my Mac. I created a simulation and got it working (also got a breadboarded version working). I then installed Eagle 6.4 with the intention of using it for wire routing. I created a new project in Eagle, created a fresh Eagle schematic, then attempted to import the LTSpice schematic (using the LTSpice icon on the schematic toolbar). After locating the correct file in the import dialog I clicked OK. I received the following error message:

Library Imported can't be found in path!

Please check: Control Panel - Options - Directories - Libraries

Add path of Imported.lbr

I have looked everwhere for this library (both on my system and on the web), but have not been able to find it. Even if I did find it, I have no idea how to configure the path statement correctly. I have also Googled various portions of the error message, looking for anyone who had the same problem. No luck. So, does someone here have any idea what I need to do to get the import working?

Thanks,

Dan Nessett

Former Member · Accepted Answer

With Jorge's gracious help, I have finally succeeded in converting the simple LTSpice model I developed into an Eagle schematic and board layout. Most of the problems were due to my inexperience with Eagle (and, frankly, also with LTSpice). However, there are a few points that I think others might find useful. Some of these are more likely to help noobees like me, but I figured, that's OK, they also need help; so I thought I would document the most important points here. First, the most "noobee" mistake I will document is failing to execute a USE command for an Eagle library that contains user defined parts before importing the LTSpice schematic. I first imported the LTSpice library containing the symbols for these parts (which in my case were symbols for the LM741 and LM386) into an Eagle library called "ImportedModels.lbr". However, I failed to execute a USE on this library before the import, which resulted in the import ulp throwing errors indicating it could not find these parts. Another noobee mistake I made was failing to assign a package to the LTSpice devices I imported from their LTSpice symbols. A third problem I ran into concerned a microphone model I used in the LTSpice schematic, which consisted of a voltage source with an internal series resistance. This confused the import ulp, which again threw an error (the specific error was - "SPICELINE" not recognized - or something like that). However, the solution was pretty simple. I just clicked on OK and the import continued on its merry way, creating a valid Eagle schematic. I don't think this is a noobee mistake, but rather a problem with the import ulp. However, it is pretty benign, so, no harm, no foul. The most significant problem I had was getting the REPLACE command to work on the devices showing up on the board view. The import ulp creates resistors and capacitor devices corresponding to the resistors and capacitors in the LTSpice schematic using a sym.lbr located in the ltspice directory under the Eagle lbr directory. The devices have a single package associated with them, which uses a surface mount technology. However, my project uses through-hole components, so I needed to convert the Eagle resistors and capacitors to use different packages. But the pin assignments in sym.lbr for the standard resistor (RES) and capacitor (CAP) are labled A and B. The pin assignments in the rcl.lbr for most resistors and capacitors use 1 and 2. So, when I attempted to replace the devices on the board with devices in rcl.lbr, it failed, informing me of the pin label mismatch. After a few email iterations with Jorge, he suggested creating a new library that modified the pin lables in rcl.lbr to use A and B lettering. I did this (first copying the rcl.lbr to a new library, which I called rcl-for-ltspice.lbr). Using this library rather than the standard rcl.lbr, the replace commands worked correctly. Changing the pin labels on the rcl devices only took a few minutes, so it really isn't much work. However, I am willing to share the rcl-for-ltspice.lbr library, if anyone wants it. Dan Nessett

autodeskguest · Answer

On 7/16/2013 2:41 PM, Dan Nessett wrote:

Hello,

I have no experience with Eagle and very very limited experience with
LTSpice (a couple of months). In fact I have little experience with
electronics hardware (I am a retired software engineer). I installed
LTSpice IV on Windows 7 running on Parallels on my Mac. I created a
simulation and got it working (also got a breadboarded version working).
I then installed Eagle 6.4 with the intention of using it for wire
routing. I created a new project in Eagle, created a fresh Eagle
schematic, then attempted to import the LTSpice schematic (using the
LTSpice icon on the schematic toolbar). After locating the correct file
in the import dialog I clicked OK. I received the following error
message:

Library Imported can't be found in path!
Please check: Control Panel - Options - Directories - Libraries
Add path of Imported.lbr

I have looked everwhere for this library (both on my system and on the
web), but have not been able to find it. Even if I did find it, I have
no idea how to configure the path statement correctly. I have also
Googled various portions of the error message, looking for anyone who
had the same problem. No luck. So, does someone here have any idea what
I need to do to get the import working?

Thanks,

Dan Nessett

--
To view any images and attachments in this post, visit:
http://www.element14.com/community/message/83322#83322

Hi Dan,

Here's what's going on.For every library or part that you use in

LTSpice, there must be a correspondance in EAGLE. EAGLE comes with the

default libraries of LTSpice already included so there's no problem there.

However if you have a custom made part from LtSpice, the library of that

part doesn't have correspondence in EAGLE's Libraries. In order to

create one open a new library in EAGLE. You'll find and LTSpice icon

there as well, left-click it and then select Import. Find the LTSpice

library you used in your design and then click OK. This will create the

parts in your open library. Save the library, into the LTSpice folder

inside lbr of EAGLE's installation directory.

Try importing the design again.

Let me know if you continue to run into issues.

Best Regards,

Jorge Garcia

Former Member · Answer

Thanks Jorge, I will forward the files to you. I assume you want the LTSpice schematic, the LTSpice subcircuit files (for the LM741 and LM386), and the symbol files for those devices. I will also include the Eable library files for the LM741 and LM386 that I imported from the LTSpice files. Cheers, Dan