Flat Patterns in Drawings

Has anybody else noticed that when you try to place a 'Flat Pattern' of a
sheet metal part on a drawing, it always places the flat pattern with the
bottom of the part facing up. This the complete opposite of how I need to
show the flat pattern on all of my parts.

As far as creating just a drawing view of the 'Flat Pattern', this isn't
really a big deal, since I can just use the 'Flip View' button to correct
this problem. Where it does pose a problem is when I bring a sheet metal
part into our Sigmanest software to laser cut a part. The parts come in
upside down just like in a drawing file. They can't be mirrored easily in
Sigmanest. So this brings me to my question;

Is there a setting for 'Flat Patterns' in Solidworks so I can set up which
side is the side of the part I want to come in face up. In my case, I would
always want the top of the part set to come in face up.

Thanks,
Richard

 

Hello Richard-
I've noticed this too.
As a work around, I create my own "Flat Pattern" view. I flatten the part,
then create a "New View" with a name like Flat Pattern For DWG.
Best Regards,
Devon T. Sowell
www.3-ddesignsolutions.com

 

Richard,

If you are using the Insert-Bends method, you can determine which side
is up based on the side that you pick as the fixed face. When a new
flat blank view is inserted into a drawing, it will place the fixed
face up and the other side is the "burr side"

If you are using the Base-Flange method, I think that you "get what you
are given". I generally won't use this method.

Personally, I would love to see soldiworks define a "burr side"
annotation or designator that made the selected face (for the
annotation) the bottom face in a drawing view and also include a
drawing callout. I believe that SW 2018 will address this. Actually I
might wager that the programmers might not even know what a "burr side"
is. But at least the toggle view option exists. Unfortunately, your
programming software does not allow you to designate up/down, so that
is an issue on their end as well as an issue with solidworks.

Later,

SMA

 

If using the Base Flange method, left click Flat Pattern, select Edit
Feature and select the fixed face.
AC

To reply via email remove all numbers from address

 

Hi Sean,

Please enlighten me, I can guess that the top of a punched part is not
burred and the bottom is?

Thanks,

Zander

 

Thanks everybody for your help.

AC, changing the fixed face in the flat pattern does the trick, thanks for
the tip.

Richard

 

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.

Later,

SMA

 

Hi Sean-Michael,

A very enlightening post. I printed this one out and saved it. This
type of information is worth it's weight in gold. Thanks again, and
feel free to continue!

Zander

 

Hi Zander -

I posted a formatted version of this last week (agreed that it might be
useful, so I "filed" it away for later). You can grab a better looking
version & has a picture of the coining at:

http://www.sheetmetaldesign.com/WhitePapers/Snippets/Burrs-Snippet.pdf

Thanks for the positive feedback.



SMA

 

Hi Sean-Michael,

Thanks, I downloaded the PDF but the picture link doesn't work?

Zander