EAGLE Central Forums
Where the EAGLE community meets. Sponsored by Stratford Digital.

Home » CadSoft Support Forums » eagle.userchat.eng » Pad size (Editing pad size )
Pad size [message #166515] Tue, 09 August 2016 22:20 Go to next message
Joseph1947
Messages: 5
Registered: August 2016
Location: Bali
Junior Member
New to eagle, I succeed to make a schematic and a board, my own library.
While trying to custom my packages pins I am getting square, round, long options
My problem is I don't understand how to get the long pad shorter than round*2
For example I want to make a pad of 70*56 mill but I am getting 112*56.
Any advice will be appreciated

Best wishes
Joe
Re: Pad size [message #166516 is a reply to message #166515] Wed, 10 August 2016 06:24 Go to previous messageGo to next message
Morten Leikvoll
Messages: 1347
Registered: November 2007
Senior Member
On 10.08.2016 00:20, Iosif Gross wrote:
> New to eagle, I succeed to make a schematic and a board, my own library.
> While trying to custom my packages pins I am getting square, round, long
> options
> My problem is I don't understand how to get the long pad shorter than
> round*2
> For example I want to make a pad of 70*56 mill but I am getting 112*56.
> Any advice will be appreciated

The builtin "long" lad is legacy stuff. You better make a round one and
draw a custom shaped polygon around it (in lib package editor). As long
as the polygon is surrounding the center of the pad, it will merge with
the pad. Of course you have to draw both bottom and top polygon pad.
Polygons can have arc sides to make the roundness you want. If you are
new to making polygons, you may need to practice this a bit.

Beware, Eagle does not support slotted holes well (yet;as by version
7.x), but there are ways around it if you know the manufacture process well.
Re: Pad size [message #166556 is a reply to message #166516] Thu, 11 August 2016 12:42 Go to previous messageGo to next message
Joseph1947
Messages: 5
Registered: August 2016
Location: Bali
Junior Member
Thank you for the advice Morten Leikvoll
Started to work on it, can make polygons already, I just have problem to save it under an other name than started with. Will continue the experiments Smile

Best wishes
Joseph
Re: Pad size [message #166557 is a reply to message #166556] Thu, 11 August 2016 13:08 Go to previous messageGo to next message
Joseph1947
Messages: 5
Registered: August 2016
Location: Bali
Junior Member
I succeed to draw two polygons I wanted as pads
I would like to save them as pads and use them for some of my packages.
Still don't understand:
* How the polygons are merging with the pad
* How to save them as pad
* How to use them when designing a new package
Will appreciate any help

Best wishes
Joseph
Re: Pad size [message #166561 is a reply to message #166557] Thu, 11 August 2016 15:46 Go to previous messageGo to next message
rachaelp
Messages: 571
Registered: March 2015
Location: UK
Senior Member
Hi Joseph,

To answer your questions in order:

1.So long as the polygon surrounds the pad then EAGLE automatically merges these. Note you need to also put polygons on the mask layers otherwise you'll have the right shape copper but the mask will only be where the actual pad is.
2. You can't save them as pads to use over and over. You create these custom pads as part of creating a footprint for a particular package.
3. See 2 above. If you want to reuse custom pads from an existing package you'll need to duplicate the existing package or copy it into a new library and then edit it to your requirements for the new footprint.

Best Regards,

Rachael

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/203535
Re: Pad size [message #166564 is a reply to message #166561] Thu, 11 August 2016 23:28 Go to previous messageGo to next message
IOSIF GROSS
Messages: 8
Registered: October 2015
Junior Member
Thank you for the replay Rachael
Will continue the experiments

Best wishes
Joe

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/203539
Re: Pad size [message #166572 is a reply to message #166564] Fri, 12 August 2016 23:55 Go to previous messageGo to next message
Joseph1947
Messages: 5
Registered: August 2016
Location: Bali
Junior Member
Very frustrated with this pad issue
I know I am new here, cant ask a simple way to make a pad?
Like defining length/width and hole?

Best wishes
Joseph
Re: Pad size [message #166573 is a reply to message #166572] Sat, 13 August 2016 07:20 Go to previous messageGo to next message
Rob Pearce
Messages: 475
Registered: September 2012
Senior Member
On 13/08/16 00:55, Iosif Gross wrote:
> Very frustrated with this pad issue
> I know I am new here, cant ask a simple way to make a pad?
> Like defining length/width and hole?
>
If all you want is an elongated through hole pad, the long hole pad
works. Its limitation is that the ratio of length to width (and offset
of the hole) are defined in the DRC rules for the board, not
individually per pad. If all your long pads want to be the same shape,
that will work for you.

If you want something more detailed or more controllable, use the
polygon method Morten recommends.
Re: Pad size [message #166578 is a reply to message #166573] Sun, 14 August 2016 06:38 Go to previous messageGo to next message
IOSIF GROSS
Messages: 8
Registered: October 2015
Junior Member
Thank you for posting CadSoft Guest.
I am not talking about individual pads
I am talking about all the pads the same in a component:
Like let say 18 Pin DIP, all pads 56/70 mill
Designing a board with long pads of 56/112 mill makes a lot of limitations to the board.
I tried the polygon, is a very time consuming approach

Best wishes
Joseph

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/203615
Re: Pad size [message #166580 is a reply to message #166578] Sun, 14 August 2016 07:06 Go to previous messageGo to next message
rachaelp
Messages: 571
Registered: March 2015
Location: UK
Senior Member
Hi Joseph,

I agree there could definitely be improvements made here. It does get quicker with practice and as you learn little techniques for doing this.

When you say the polygon approach was time consuming, what was your process? It'll be slower for the initial pad within the package but once you have done one pad its just a matter of setting the grid to the pin pitch and then doing a group copy of all the parts of the custom pad and pasting it for each of the pins on the first side, then setting the grid to the pitch between the two rows of pins and doing a group copy and paste of the whole first row to create the remaining pins. Then type NAME and press return and go round clicking each pin and naming it correctly to ensure all the pins are in the correct order.

Best Regards,

Rachael

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/203587
Re: Pad size [message #166587 is a reply to message #166580] Mon, 15 August 2016 00:58 Go to previous messageGo to next message
Joseph1947
Messages: 5
Registered: August 2016
Location: Bali
Junior Member
Thank you for the replay Rachaelp
I have done what you are proposing and made an 18 pin package with pads of 70/56 mill
1. I didn't succeed to copy the pad, top, bottom, top solder mask, bottom solder mask polygons all together so I done it one by one
2. In the saved package, is still see the polygons and the pad and not a pad of 70/56 mill
3. Tried to replace the package of the PIC18F1847-I/P in my drawing with my new package, followed the manual step by step with no success.
4. Tried to add the package to the PIC18F1847F-I/P without success.
In general, the manual assumes that you know a lot of things already, don't have step by step procedures.

I am using WinQcad for many years, was/I am very happy with the software but I suppose you know they existence ended a few years ago and I found Eagle to be the most affordable and serious medium level SCH/PCB software, also used by Elelent14 and SpakFun.
I have a total of some 50 Packs I am using and would like to have them in Eagle, most pads are 70/56 mill and round 56 mill (given by Eagle)

Best wishes
Joe
Re: Pad size [message #166589 is a reply to message #166587] Mon, 15 August 2016 08:21 Go to previous messageGo to next message
rachaelp
Messages: 571
Registered: March 2015
Location: UK
Senior Member
> IOSIF GROSS wrote:
>
> 1. I didn't succeed to copy the pad, top, bottom, top solder mask, bottom
> solder mask polygons all together so I done it one by one
You need to group them with the group tool first, then go into copy mode, right click on one of the items in the group and select 'copy group' from the menu.
> IOSIF GROSS wrote:
>
> 2. In the saved package, is still see the polygons and the pad and not a
> pad of 70/56 mill
When you say in the saved package, where are you viewing this? If you've just created this package in the library you should see it in the library browser but you need to do a few more things to get it associated with the actual component.
> IOSIF GROSS wrote:
>
> 3. Tried to replace the package of the PIC18F1847-I/P in my drawing with my
> new package, followed the manual step by step with no success.
> 4. Tried to add the package to the PIC18F1847F-I/P without success.
> In general, the manual assumes that you know a lot of things already, don't
> have step by step procedures.
Have you created the new package in the same library as your PIC part that you are using? Have you added that package as a variant to the part itself so it's available for selection? If you haven't then this is your problem. The procedure to do this is as follows:
1. Open up your library containing the PIC and your new package (they must be in the same .lbr file)
2. Open the PIC device to view its symbol and packages
3. Click on the 'New' button in the bottom right.
4. Single click on the new package you have created from the list.
5. Give this new package a variant name.
6. Click on 'OK'. Your new variant will appear in the list on the right hand side but it won't have a green tick against it.
7. Double click on your variant in the list.
8. Assign the pins in the resulting dialog by using the 'copy from' drop down to select the mapping from the existing part or manually mapping them yourself if your pin numbering doesn't quite match the original.
> IOSIF GROSS wrote:
>
> I am using WinQcad for many years, was/I am very happy with the software
> but I suppose you know they existence ended a few years ago and I found
> Eagle to be the most affordable and serious medium level SCH/PCB software,
> also used by Elelent14 and SpakFun.
> I have a total of some 50 Packs I am using and would like to have them in
> Eagle, most pads are 70/56 mill and round 56 mill (given by Eagle)
EAGLE has it's usability quirks and when you are very familiar with another tool and know you can do something quickly in that tool then it can be frustrating. It does get easier and once you get used to the methodology used by EAGLE it does actually become relatively quick for a lot of things. But there is a learning curve and it take patience and practice. Keep at it and you'll get there, and if you have any more questions just ask :-)

Best Regards,

Rachael

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/203670
Re: Pad size [message #166598 is a reply to message #166589] Mon, 15 August 2016 09:39 Go to previous message
IOSIF GROSS
Messages: 8
Registered: October 2015
Junior Member
Thank you for the post Rachael
I copy your post to my computer and will do as you advised
In any case, The pic16f1847 is un my new 1LME.lib and the package is in my new 1LME library under the Packages

Best wishes
Joe

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/203618
Previous Topic: EAGLE est génial sur des choses compliquées mais des simples...
Next Topic: Future of Eagle
Goto Forum:
  


Current Time: Mon Jun 26 07:12:51 GMT 2017