why so
What is the problem
Hi Arif,
the reason why you get two different weights based on the status of the sheet metal part (folded or unfolded) is that the actual geometry is different. The SOLIDWORKS weight calculation is based on the actual volume of the body and this is in fact in most cases different (in your example the volume of the bends in the bended state is bigger than the volume of the flattened bends). In real life both weights are likely identical since the material gets stretched/compressed in the bend areas. However this is not possible to simulate in SOLIDWORKS and therefore we are using a simplified model with a constant material thickness in the bend area (what usually leads to a bigger mass for the bended body).
This is why we introduced two different mass options for sheet metal parts. There is the part mass as it is usually used and there is the "flattened mass" which refers to the unfolded body even though the folded body gets displayed:
I.e. if you want to use the "Flattened Mass" as the common mass (i.e. to display the mass on a drawing) you can select "Flattened Mass" from the dropdown. Means that we are unfolding the part in the background in order to get the unfolded weight that gets used in the part properties.
Hope this explains the behavior.
Kind regards
Frank SOLIDWORKS Product Definition Team
Frank,
It totally makes sense; however, it's like there are only flanges and both are flatterned without any extra feature (from the image on his post)
Hi Christian,
the point is that the volume calculation is influenced by i.e. the k-factor. If you use a k-factor that is smaller than .5 the length of the developed length will become shorter than it is in the folded part and that will make the folded body "heavier" than the unfolded body. But if you use a k-factor bigger than .5 you will get a longer developed length and the flattened body will be actually heavier than the folded body. But since quite a lot of users are using k-factors between .3 and .5 there is usually the flattened part lighter than the folded body.
Kind regards
Frank
SOLIDWORKS Product Definition Team
In theory, the volume should remain the same before and after folding. Where's the "extra" volume from?
Hi Christian,
yes, in the real world the weight should be identically but in SOLIDWORKS the weight will change based on the bend parameters. As I said, the volume of the bend in the folded state might be bigger than the volume in the unfolded state.
Kind regards
Frank
SOLIDWORKS Product Definition Team
In the CAD world, a sheet 5mm thick with a bend that has a 5mm inside radii would have an outside radii of 10mm.
In the real world, a sheet 5mm thick with a bend that has a 5mm inside radii would have an outside radii of 12mm or so.
The volume in the corners of the "eyebrow" is the difference.
Use K-Factor of .5 and CAD world = real world (only not really).
Hi Frank,
I don't see the SW-FlattenedMass property in my sheetmetal parts (using 2016 SP5)
Hi Ian,
this is odd since we implemented the "Flattened Mass" option with 2016. I just double checked and created a new part from scratch and it offers the "Flattened Mass" as possible value. Not sure what is going on in your example.
Kind regards
Frank
SOLIDWORKS Product Definition Team
Hi Frank,
contacted our VAR and he pointed out the problem is our templates are out of date. It would be good if Solidworks notified when templates have to be replaced in new versions, or better still updated existing templates when they are saved in new version (I checked, opening and saving our templates in 2016 does not fix this).
Ian McLean wrote:
contacted our VAR and he pointed out the problem is our templates are out of date.
Ian,
Did this fix your weight discrepancy?
What specifically did your VAR tell you was out of date?
Hi Rick,
Flattened Mass was introduced in 2016 and it appears that cut list properties are stored in the file template. So if a template that was created in 2015 or earlier is used to create a part, it will not show the flattened mass cut list property in the list.
You can check the template creation date by right clicking on one of the template base features, e.g the default planes and selecting 'properties'. The date here is an indication of when the template was created.
Saving the template in a later version does not change the template date of creation, and the architecture of this template remains the same to prevent breaking features that are already created.
Hi Ian,
I am sorry to hear that you have to create new templates. I was checking my old files and it looks like there is a difference between files that were created before the 2013 release (because those won't get the "Flattened Mass" option) and files created with 2013 and newer (these seem to be compatible with "Flattened Mass").
We did a huge architectural change for sheet metal components with the 2013 release which was required in order to improve multi body sheet metal quality. It looks like quite some (sheet metal) features that we did after 2013 might not be compatible with files created prior to that release. For this architectural change there is currently no save way to upgrade files created before and therefore we did not pursue this solution.
Unfortunately those incompatibilities happen even though we try very hard to avoid them if possible and in the majority of cases we succeed in doing so. But in some few cases there are serious changes required that are not compatible with legacy components but nevertheless have to be made for a better future quality.
However we obviously missed out on conveying the information that "Flattened Mass" is not available for components created prior to 2013 what is bad and something we can improve in the future.
Kind regards
Frank
SOLIDWORKS Product Definition Team
Can you post your model here - I tried to to model a sheet metal part and the weight remains the same before and after flattern