Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

How to create a component/footprint…

Status
Not open for further replies.
C

chaki

Newbie level 1
Joined
Aug 31, 2012
Messages
1
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,297
Hello everbody,
I’m changing my status from an interested reader to an interested writer, because I haven’t found an answer to my question about creating a component (footprint). I hope I can learn from your experience…
Following question:
I do have a datasheet (let’s say it is a capacitor or something) and all of the dimensions are in mm (for example lead spacing = 7.5mm).
If I create my new component and I want to do this in mil, should I convert these 7.5mm to 295.28mil, 295mil or to 300mil. What kind of specifications would make an experienced designer/layouter.
Thanks for helping me…
 

It depends on the capabilities of your tool. If your tool has a resolution of .01 mil, I would use 295.28. There's no reason to throw away accuracy; what would you gain?
 

chaki said:
Hello everbody,
I’m changing my status from an interested reader to an interested writer, because I haven’t found an answer to my question about creating a component (footprint). I hope I can learn from your experience…
Following question:
I do have a datasheet (let’s say it is a capacitor or something) and all of the dimensions are in mm (for example lead spacing = 7.5mm).
If I create my new component and I want to do this in mil, should I convert these 7.5mm to 295.28mil, 295mil or to 300mil. What kind of specifications would make an experienced designer/layouter.
Thanks for helping me…
Click to expand...

dont worry if you re using eagle then I did those videos especially for people who have the same issue i will show u how to create

a DIL dual in line package footprint in two parts videos

part 1

https://www.youtube.com/watch?v=veOCJDua7bg&feature=plcp

part2

https://www.youtube.com/watch?v=gUdRam-DOSM&feature=plcp

In a second video I will show you how create a So small outline footprint

https://www.youtube.com/watch?v=vJ9wje8hXAM&feature=plcp

and then how create the device

https://www.youtube.com/watch?v=8OM7uSXerFI&feature=plcp


you can follow me either on my youtube channel or in my facebook page

www.facebook.com/electronicsforal

Thank you
 

With respect, I followed your SO package video, but that is really _not_ how to create a package. There were many mistakes - you don't need to pick the 'closest' sized pads, you can specify the _exact_ pad size, and I really don't think manually moving pads with a mouse pointer is a good way. Also, you picked the wrong width when you placed the pads on the other side of the package.
Basically, get used to using the command line in EAGLE, and use the SMD command, and type co-ordinates (absolute or relative) on the command line. Also, you don't need to type the component name (think about what you'd need to do if you had hundreds of different devices, each with the same package - would you create hundreds of packages?). You can use a code ">NAME" and ">VALUE" to get EAGLE to automatically assign the corrent component identifier and value. Most of this is in the EAGLE tutorial doc.
 
sky_123 said:
With respect, I followed your SO package video, but that is really _not_ how to create a package. There were many mistakes - you don't need to pick the 'closest' sized pads, you can specify the _exact_ pad size, and I really don't think manually moving pads with a mouse pointer is a good way. Also, you picked the wrong width when you placed the pads on the other side of the package.
Basically, get used to using the command line in EAGLE, and use the SMD command, and type co-ordinates (absolute or relative) on the command line. Also, you don't need to type the component name (think about what you'd need to do if you had hundreds of different devices, each with the same package - would you create hundreds of packages?). You can use a code ">NAME" and ">VALUE" to get EAGLE to automatically assign the corrent component identifier and value. Most of this is in the EAGLE tutorial doc.
Click to expand...

Really appreciated your critics sky-123 eventhought if this (not appropriate technique lets say and it is) had been working for me, any other constructive critics like those
about the (the many mistakes) you,ve told about in your post
are strongly welcomed if there are any others critics about the dil foot print or the other videos they will be also appreciated

Thank you sky-123
 

No problem, these things take ages to figure out with EAGLE the first time round. EAGLE isn't easy, but it is quick to use via the command line once you're used to it. So, if you do get round to creating a video showing the command line, I think it would help lots of other users.

Here is an example of a script that could be entered as command lines in EAGLE - this will generate a SO-8 SMD package.
(I auto-generate scripts using some simple program I wrote, but this just saves a bit of time - not essential).
This is just to help explain what some of the commands look like - if manually creating a SO-8, I would probably use the SMD
command shown in the example below for all the pads, and then maybe manually place the outline with the mouse.
Good to have Windows Calculator nearby when using the command line.

Code: 
grid mm
grid 1
set wire_bend 2
layer tPlace 
wire 0.127000 (-2.500000 -1.619000) (2.500000 -1.619000)
wire 0.127000 (2.500000 -1.619000) (2.500000 1.619000)
wire 0.127000 (2.500000 1.619000) (-2.500000 1.619000)
wire 0.127000 (-2.500000 1.619000) (-2.500000 -1.619000)
circle 0 (-2.000000 -1.119000) (-1.700000 -1.119000)
set size 1.27
layer tnames
text >NAME (-2.500000 -5.470000)
layer tvalues
text >VALUE (-2.500000 4.200000)
layer top
smd 0.762000 1.200000 '1' (-1.905000 -2.600000)
smd 0.762000 1.200000 '2' (-0.635000 -2.600000)
smd 0.762000 1.200000 '3' (0.635000 -2.600000)
smd 0.762000 1.200000 '4' (1.905000 -2.600000)
smd 0.762000 1.200000 '5' (1.905000 2.600000)
smd 0.762000 1.200000 '6' (0.635000 2.600000)
smd 0.762000 1.200000 '7' (-0.635000 2.600000)
smd 0.762000 1.200000 '8' (-1.905000 2.600000)
 

IMO if the dimensions are in MM then create the component in MM and make it exactly as the datasheet says it should be rather than nearly there by converting it.

Its only a unit of measurement, I do not know of a CAD package that does not let you use both mm & mil/thou
 

sky_123 said:
No problem, these things take ages to figure out with EAGLE the first time round. EAGLE isn't easy, but it is quick to use via the command line once you're used to it. So, if you do get round to creating a video showing the command line, I think it would help lots of other users.

Here is an example of a script that could be entered as command lines in EAGLE - this will generate a SO-8 SMD package.
(I auto-generate scripts using some simple program I wrote, but this just saves a bit of time - not essential).
This is just to help explain what some of the commands look like - if manually creating a SO-8, I would probably use the SMD
command shown in the example below for all the pads, and then maybe manually place the outline with the mouse.
Good to have Windows Calculator nearby when using the command line.

Code: 
grid mm
grid 1
set wire_bend 2
layer tPlace 
wire 0.127000 (-2.500000 -1.619000) (2.500000 -1.619000)
wire 0.127000 (2.500000 -1.619000) (2.500000 1.619000)
wire 0.127000 (2.500000 1.619000) (-2.500000 1.619000)
wire 0.127000 (-2.500000 1.619000) (-2.500000 -1.619000)
circle 0 (-2.000000 -1.119000) (-1.700000 -1.119000)
set size 1.27
layer tnames
text >NAME (-2.500000 -5.470000)
layer tvalues
text >VALUE (-2.500000 4.200000)
layer top
smd 0.762000 1.200000 '1' (-1.905000 -2.600000)
smd 0.762000 1.200000 '2' (-0.635000 -2.600000)
smd 0.762000 1.200000 '3' (0.635000 -2.600000)
smd 0.762000 1.200000 '4' (1.905000 -2.600000)
smd 0.762000 1.200000 '5' (1.905000 2.600000)
smd 0.762000 1.200000 '6' (0.635000 2.600000)
smd 0.762000 1.200000 '7' (-0.635000 2.600000)
smd 0.762000 1.200000 '8' (-1.905000 2.600000)
Click to expand...

It an excellent idea in deed I will post some videos about src and ulp in the near future and replace the previous videos
 

Use IPC-7351 as your guidance and go metric, most modern components are.
Me I do my symbols graphicaly on screen, or use a ipc-7351-wizzard where possible, doing them graphicly ith the correct grid has always worked for me.
 

Like sky_123 I often do them by typing in co-ordinates. I guess it depends on the tool you use. In Eagle the grid is the same in x and y directions so you cannot always pick a grid that suits both. One way round that for a quad pack is to place one row along one axis graphically using one grid then change the grid and move it to the right place.

Keith.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top