Need Eagle help

[yoshimitsuspeed]

Is anyone here familiar with Eagle and also the F360 integration? 
I am very new to Eagle and trying to figure out what would be the best way to design some components. 
The first is an assembled PCB that will be going on the main PCB. 
https://www.diyautotune.com/product/microsquirt-module-v2-2/
Using these headers. 
https://www.diyautotune.com/…/microsquirt-module-hardware-…/

Now the headers are in Eagle but I will need to precisely position them relative to each other and to the mounting holes. 
From what I have gathered about Eagle it looks like this would be a massive PITA. 
Could I lay it out in F360 then import it into Eagle? Or is there a fast efficient way to do this in Eagle?

I will also be adding this header. 
http://perfecttuning.net/…/toyota-supra-7m-gte-2-rows-52-pi…

Which needs to be very precisely positioned on the board.
I modeled the circuit board in F360 off a 3D scan and not really knowing what I was doing I modeled the holes for this header into the circuit board. They are perfectly located but it looks like I need to have it in the Eagle library so I can use it for a schematic and run circuits to it. Or is there a way to run circuits to holes modeled in F360? If not then what would be the easiest way to design this in Eagle? Again from what I have seen it looks like it would be a nightmare to design in Eagle and even once I did I don't see any way to dimension it's position.

[havlicek6TH3H]

Hi,

you can precisely position parts in Eagle. Just place the component on the board, switch grid to prefered units (command - grid 1 1 mm for example) and then click on the info button, click on part ant there is a position of a part so you can change it as you want. 

It will need some math, to calculate position of components but it should be ok. (It´s little bit like in old AutoCad R14 )

[rachaelATWH4]

---

@yoshimitsuspeed wrote:

Is anyone here familiar with Eagle and also the F360 integration? 
I am very new to Eagle and trying to figure out what would be the best way to design some components. 
The first is an assembled PCB that will be going on the main PCB. 
https://www.diyautotune.com/product/microsquirt-module-v2-2/
Using these headers. 
https://www.diyautotune.com/…/microsquirt-module-hardware-…/

Now the headers are in Eagle but I will need to precisely position them relative to each other and to the mounting holes. 
From what I have gathered about Eagle it looks like this would be a massive PITA. 
Could I lay it out in F360 then import it into Eagle? Or is there a fast efficient way to do this in Eagle?

I will also be adding this header. 
http://perfecttuning.net/…/toyota-supra-7m-gte-2-rows-52-pi…

Which needs to be very precisely positioned on the board.
I modeled the circuit board in F360 off a 3D scan and not really knowing what I was doing I modeled the holes for this header into the circuit board. They are perfectly located but it looks like I need to have it in the Eagle library so I can use it for a schematic and run circuits to it. Or is there a way to run circuits to holes modeled in F360? If not then what would be the easiest way to design this in Eagle? Again from what I have seen it looks like it would be a nightmare to design in Eagle and even once I did I don't see any way to dimension it's position.

---

Hello,

Fortunately is it quite easy to place things in exact positions or exact positions relative to something else.

So, if you know (or can easily calculate) the exact positions of each of your connectors, lets call them CON1 and CON2, and lets just say they need positioning at x=30.00m, y=20.00mm and x=50mm, y=30.00mm respectively. You could issue the following commands.

GRID mm;
MOVE CON1 (30.00 20.00); LOCK CON1;
MOVE CON2 (50.00 30.00); LOCK CON2;

If you don't know the exact positions but you know their relative positions to another object then this will need altering slightly to start from the known object position. You could of course calculate the exact positions but there is no need.

So lets say we have an object at x=15.00mm, y=10.00mm. So this would make the above locations relative to the known object (we're reverse calculating just for the sake of the example) of CON1 and CON2, x=15.00m, y=10.00mm and x=35mm, y=20.00mm respectively. To position these before using relative positioning you can do the following:

GRID mm;
MARK (10.00 10.00);
MOVE CON1 (R 15.00 10.00); LOCK CON1;
MOVE CON2 (R 35.00 20.00); LOCK CON2;

Note the addition of the MARK command placed at the location of the known object, and the addition of the R in the co-ordinate specification to denote the position specified it relative rather than absolute.

Now, I have written a ULP to help speed this up somewhat which is part of my EAGLE ULP Utilities library. If you go to my blog on Element14 you will find the link to the GIT repository:

EAGLE ULP Utilities Library

Most of the utilities are documented there, unfortunately the one you want hasn't been documented yet. If you download the repository and add the folder containing the ULP into the directory specification for your ULP path then you can run the following command to install the needed tool:

run moveTools --install

Then you can right click on a component and you will see three new options, "Set Mark...", "Move To...", and "Move Again...". You can use the first of these to set the MARK as shown above and the second option to perform the move. There are a few options you can choose on the resulting dialog, make sure you understand all the options, especially how it deals with updating the MARK as this may or may not be what you need to do depending on how your relative positioning is specified.

Let me know if you need any more info!

Best Regards,

Rachael

[rachaelATWH4]

One thing to note... EAGLE v.8.5.0 seems to have a bug which has broken ULP running from the right click context menu. I know they are working on fixing it and I expect it'll be fixed in an 8.5.1 release pretty soon so I would suggest if you need to use my ULP (and you should feel free to make use of my Utils library in general) then I would advise you use EAGLE v8.4.3 for now until they release the fixed version.

Best Regards,

Rachael

[yoshimitsuspeed]

I posted this in the Fusion 360 forum in hopes I could use F360 in as much of the design process as possible but someone frikken moved my post. 
Thanks for the responses and I appreciate the input. The responses were pretty much what I expected. Something that I could design in F360 in 10 min sounds like it could be an hour or more of stupid little calculations and compromises. I am going to take this back to the F360 forums and see if there is any way to do some of the design in there but thanks for the input and I will likely be back with more questions. 

[yoshimitsuspeed]

@rachaelATWH4

In that blog you mention importing DXFs
Can I just sketch out the holes and pin locations in F360 and then just designate the pins in Eagle? 

[rachaelATWH4]

---

@yoshimitsuspeed wrote:

@rachaelATWH4

In that blog you mention importing DXFs
Can I just sketch out the holes and pin locations in F360 and then just designate the pins in Eagle? 

---

Using the ULP's in my ULP Utilities Library you should be able to do what you are wanting to do very quickly and yes you could create a DXF with all the holes and connector positions located and import that into EAGLE and it would help speed things up.

You likely can use F360 more directly but the EAGLE<->F360 link, while a hugely important and great feature, isn't without it's issues at the moment and you might find it easier to use a more traditional approach.

So (use 8.4.3 as 8.5.0 has some issues which broke some ULP features) install the moveTools.ulp and addHole.ulp into your EAGLE using:

run addHole --install

and

run moveTools --install

Now, import your DXF. Use circles to represent any holes in your board and make them the correct size. Also use circles to set the centre point of your connectors. If your connector components have been created not centred on the origin then if it were me I would correct that, but you can also do your DXF so the position markings are relative to where you know the origin point is in the connector parts.

So... In the board, File->Import...->DXF... and follow the instructions in that import process.

Now, for each of the locations in the board which require a hole, locate the corresponding hole in the DXF layer (make sure it's visible) and right click on it and choose "Place Hole (Non-PT)..." or "Place Hole (PT)..." depending on whether your holes should be plated or non plated.

Now, on one of the circles representing your connector origin, right click and place hole (this is a temporary step until I update the moveTools.ulp!).

Now right click on the hole you just placed and choose "Set Mark...". You can go ahead an delete the hole now, making sure to leave the mark in place.

You can either right click on you connector and use the "Move To..." option to move the connector to x=0, y=0 relative to the mark or issue the command:

MOVE CON1 (R 0 0);

Where CON1 is substituted for the reference designator of your connector.

Rinse and repeat for any other components you need to place exactly.

I'm pretty sure I could place a lot of components quickly and accurately using this method. It definitely shouldn't take an hour, no more than a minute or two once you have your DXF from F360.

If you have any issues or need further help feel free to ask!

Best Regards,

Rachael