PADS ASCII IMPORT BUG - PCBLIB ORIGIN OFFSET

Altium Bug Crunch
http://bugcrunch.live.altium.com/#Bug/4651

This bug was found in AD14.3.14  (latest release). 

Note AD14.2.5 Does not have this problem.

Most likely this bug was introduced into AD14.3.14 while making these enhancements.



Source: http://techdocs.altium.com/pages/viewpage.action?pageId=235578

Note the origin data error will be passed to the pick and place file data.

Steps to re-create the bug:

Download and Import this PADs ascii file INDC3225X280N.asc in to Altium using the import wizard.

Then make pcblib library. 

As shown below the pcblib file created from the pcbdoc has an origin offset.




Step by Step:

Import the PADs ASCII file at the link provided above.

click on images to view

After importing the PADS ASCII file, zoom to the center of the target (crosshairs) and note that the origin is correctly centered in the target.

Also a quick check of the pads properties shows the pads are properly centered about the origin. As shown below the left pad is located at X -1.47mm, Y 0mm

Also the right pad is correctly located at X 1.47mm, Y 0mm

So far everything is correct. 

Now let's create a pcblib from the imported PADs ASCII file (the Altium pcbdoc) and zoom in to view the origin in the PcbLib.

As shown below there is an offset error in the origin.

This is serious flaw for anyone who is importing PADs asc data and generating Altium library parts. 

This incorrect origin data will be passed to the pick and place file data. 

Also the origin error will adversely affect part placement base on the part's origin.

Checking the Left and Right Pad X & Y properties also shows there is and offset error.

Left pad X -1.4827mm,  Y -0.0127mm

and the right pad X 1.4573mm, Y -0.0127mm

Work-arounds:

1. Manually move the origin in pcblib to center of the target (crosshairs).
2. Select Edit > Set Reference > Center

Summary:

Be aware that when importing PADS ASCII data that until this bug is fixed you may need to move the origin in the pcblib files generated after using the import wizard and creating pcblib libraries.

If you have an interest in seeing this bug fixed, cast your vote at:
http://bugcrunch.live.altium.com/#Bug/4651

That's It

Release Notes for Altium Designer Version 14.3 | Online Documentation for Altium Products

Here's what changed in AD14.3.14 (released on Aug 25, 2014)

Release Notes for Altium Designer Version 14.3 | Online Documentation for Altium Products:


'via Blog this'

Polygon Cutouts - Altium Discussion Forums

Polygon is wrongly poured over polygon cutout - Altium Discussion Forums:

Workaround for Polygon Cutouts in AD14.3.14

"I tried this with a new, blank board.

I placed a polygon and then, a polygon cutout inside. The polygon cutout is not working. Then i have changed it to board cutout, and it works as expected. When i change it back to polygon cutout again, it works !!!

By the way, I found out, that it works, if you move the polygon."

Source: 
http://forum.live.altium.com/posts/204342/573029

'via Blog this'

Rooms - For Clearance Exceptions

Rooms are useful for creating exceptions. 

For example this Ethernet design called for 18 mils of clearance from the differential pairs to adjacent copper pours.

The diff pair nets were placed in class and a clearance rule was created to hold polygon pours back 18 mils.

click on images to view

This took care of the 18 mil (~3 x W) copper clearance requirement.


However as shown above, now there is a clearance error where the differential pairs connect to U500.

We can use a room to define a clearance exception for the differential pair at U500.

Define the Room

Design > Rooms

Tip: Use Shift + Click to Select an Existing Room

Tip: Select a handle on the Room > Drag Handle > Tab Key

Take note of the settings used for the room above, specifically:

Name RX_TX_ROOM

Not InComponent('U500') 

'Keep Objects Outside' 


Clearance Rule

That's It.

Drill Chart Properties

Selecting the new Drill Chart Properties can leave you frustrated.

Right Click the upper left handle in the table's corner to bring up the properties dialog.

Good luck, it's kinda of random that you will bring up drill table properties, more often than not you end up selecting a track in the table's frame.

Please let me know if you have a better method.

That's it.