Showing results for 
Search instead for 
Did you mean: 
Showing results for 
Search instead for 
Did you mean: 

The PTC Community email address has changed to Learn more.

Sheet metal Blank Issue


Sheet metal Blank Issue


I have some doubt related to Sheet metal. While Creating sheet metal drawing using with material grade AISI 1018(MS), there is variation while comparing to creo sheet metal bending dimensions with manufacturing (output dimensions) How this variation happened? Because Dimension variation nearly 4.0 to 5.0mm more when comparing software to real time manufacturing , Can u people guide me or explain me how it happening?


For Example :

Blank Dimensions  for both In drawing & Real time manufacturing : 97.3/97.5mm

In Drawing  (after bending) - Width :55.0mm x Height : 25.0mm , But 

In Real time manufacturing (After Bending) - Width : 59.0mm x Height 25.0mm.

How ?


Bending :

In Drawing bending done in number stage or number stroke type( Because we never get blank dimensions while use forming tool type in creo)

In Real time manufacturing done in forming type (Single Stage or stroke)


Please guide us !



A couple things-

Assign the correct bend table for the material, table2.

Model the part bend radii to be the same nominal radii that correspond to the V-Die width you are using.

Folks who supply tooling for bending have bend charts that list these things.

After bending, verify your bends are 90 degrees and each wall is the correct height.

If you do all of the above, you should be just about perfect, assuming your bending process is "air bending" and you are using a recommended V-Die width for your material thickness and your punch radius is not too small.

With Air-Bending, V-Die width should never be used to produce a bend radius (inside radius) that is smaller than the material thickness for air bending, then you are coining and will need longer blank.

If your bend process is "coining" or you are using "Rolla-V", correlation is going to be more involved.

23-Emerald II

Be sure the K-factor value for material reduction is proper for your material. 

The values in Creo by default are not correct for most materials.


You may need to experiment with some samples to get a true correspondence between manufacturing and Creo.


I know where I used to work, when we installed Wildfire, the default K-factor was set to .5 by PTC. We had been using Unigraphics for years and knew that a .43 K-factor was what we needed for our materials and processes. In this case it was easy to set as we know what the value was that we needed.

23-Emerald II

Is this part being formed in a single operation, drawing process, or bent on a press brake, one bend at a time?


The drawing process may be stretching and thinning the 25mm wall thickness on each side and thus 'forcing' extra material into the 10mm ear lengths.

One more observation-

Your drawing shows 2 different bend radii, R1 and R0.5.

The bend radius is a function of the V-Die, to bend this part per your drawing would require using 2 different V-Die widths, is this the process being used?

To obtain correlation between Creo and the bending process, your models have to be modeled with the same bend radii that the bending tooling produces. Conversely, the bending tooling must be chosen to produce the bend radii specified in Creo.

I have done thousands of parts through Creo and have had excellent results using Creo flats, usually within .005".

The only adjustment I have had to make to the default settings were for 10 gauge stainless steel.


Is the material thickness?

This is critical for getting the flat pattern right.


With 1mm thickness, I get a flat length of 99.7 with .5 Y-factor. changes to 99.43 with .43 Y-factor.