Hi Zander -
When punching anything there is a burr on the "part" and the "scrap" and the direction of these two is always opposed.
Part burr is generally down and the scrap burr is generally up.
For most all punching applications, the part's burr is down because the punch that creates the part is in the upper portion of the punching machine generally called the "ram" (punch press, turret press, etc).
This does not disqualify a burr from being up like in the case when the part is punched down through a die (matrix). There are also conditions where a part's burr is "reversed", for example when the majority of a part is punched in a progressive die (burrs down) and then the part is taken off the carrier strip by being punched thru the lower die. This is not generally a good practice for other reasons not covered here.
In most of the cases, burr direction is down and it is a good practice to indicate this condition and to show a flat blank with the burr down. This is sometimes refered to as "viewed thru the upper" (ram). Alternately, "Burr Direction" is opposed to another thing which is called "Punch Direction". When the term "Punch Direction" is used, it implies that the burr will be on the OPPOSITE side.
In general, part burrs are considered acceptable within 10% of the part thickness, hence, a part of .060" thickness will generally be allowed to have burrs of up to .006" high.
When designing parts for high production (i.e. tooled) it is a good practice to indicate "Burr Side" or alternately "Punch Direction". It is also a good practice to form burrs to the "inside" of a bend particularly the smaller it gets. Because the "sheared" portion of a cut sheet metal part has a high burnish, cracks are less likely to form on the outiside of a bend (not to be confused with orange peeling). Burrs are also often formed to the inside of an enclosure for human safety reasons.
It is important for designeres to consider the significance of burrs in a high production setting and the divergence of punched features from the ideal model. Generally, none of the cut edges on a sheet metal part is square to the faces of the part.
A cut edge has Roll-Over (about 5% of the thickness), Shear (about 30% of the thickness), Break (The remaining % of the thickness) and Burr, potentially up to 10% of material.
It is generally not economically viable to have parts that are 100 burr free in any settings. Common strategies for burr management are:
1 - Know the burr liability and control the burr side by a callout based on the context of ones design. (cheapest option)
2 - Secondary op tumbling (not generally bad for smaller parts and a good option for parts handled by humans). This may be done in the flat state or in the formed state.
3 - A sanding process known as "Time Saving" - this is where the parts are run between sanding belts - not to bad, but this must be done in the flat state. The edges are still a bit sharp, but have no protruding burrs. Another thing similar to this is called DQ sanding and gives a circular looking surface.
4 - Burr flattening within tooling. This is often accomplished by a hardened bottoming block in a progressive die or sometimes is a hidden extra of a forming process that "bottoms" on the part, but only in the area that is contacted in a tool. Again, this is a "no protrusion" item like the above and is not relatively costly (only needs tooling real estate) since it is part of the progressive stampig op.
5 - Coin Burr within tooling - This is where a part edge is actually coined. Generally, a countouring die is needed and this die has a .015 radius with a 10 degree "lead-in" and an upper anvil block that coins the burr. This is a true safety edge and will generally not cut people, but it is expensive to implement in tooling. If this type of feature is used, a straight edge will be less espensive that an irregular contour. A straight edge can be ground much like a conventional form block profile (I.e. it is a "cylindrical" body), but a contoured edge must generally be hard machined with carbide (blocks are hard A2 or similar tool steel - rc58-60) or conventional EDM'd. Alternately these are finished soft and the distortion engendered by heat treating is tolerated. In any case, implementing a coin burr process gets expensive fast. Additionally, it is common practice to implement a "balancing" coin to keep the part from pushing away during coining (inevitable but a balance keeps the coin crisp along a long edge fopr example).
6 - Electropolish - In this process the part is dipped in a conductive vat of stuff and electrically polished (kind of electrically eroder). The burrs generally die and the part gets a higher sheen.
7 - Human Deburring Labor - Be prepared to pay dearly . . . In any case, that's a little ditty on burrs.
In a low production environment (laser), laser slag is often present were burrs would be, but it is usually remedied by Time Saving. In a low to medium (turret press) burrs are present and commonly there are "spike burrs" that come from line-to-line shearing.
Personally, I wish that solidworks had a "model embedded" burr side annotation, but doubt that it would ever make it into the program - it's too much of a "real world" need (Sarcastic Smile) .
Short answer - be aware that burrs are there and thay can effect your design if uncontrolled.