I am new to Solid Edge but I have touch to some other CAD. I work in sheet metal and i need a way to quickly calculate de neutral fiber of a bend. We have an in house chart and i manage to put it in variable into my basic piece template. We get .STEP files and convert them into sheet metal for laser and bending operations. So basically I need a way to get the bend radius from somewhere in Solid Edge. What I am missing is the "somewhere" part. I dont want to enter it by and as I am better entering the neutral fiber at this point.
I tought using the bend table that is generated after you transform a solid. I can't locate the bend radius variable into the table.
This method will only be use for simple part with equal bend radius all around the part. This should cover around 90% of the job. I have include what I got so far as some screenshots.
Solid Edge is in french here so sorry about that. Anyway I am pretty sure you guys can navigate it eyes closed.
Don't worry about guiding me in your English version. I should be able to follow.
Also, If there is anywhere a list of all variables in ST9, it might be very handy.
I don't deal with enough sheet metal, so I end up using the standard numbers. There are plenty of Sheet Metal experts on this forum that I'm sure will chime in the next time they are online.
But, I think if you research the Gage Table [gagetable.xls] usually located in your preferences folder, you may find the level of control you are looking for. You also may have to look at the Material Table, Gage tab.
as answered by @swertel already,
it is not difficult to define your sheet metal bending properties.
The easiset way to do so is - IMHO - via the variable table of Your SE sheet metal part.
Enter the variable table either via extra - variables
or You also can use Your right mouse buttton somewhere in graphics where You will find a link to the variable table.
Here You cann see the entries for Material Thickness, Bend Radius and very important the Neutral Factor
At this point, sorry for the German interface!
Changing this values will have effect for Your sheet metal part
Only to mentione it, the neutral factor specifies where the neutral zone will be within the material thickness.
A neutral factor of 0.33 points out that the neutral zone is at 33% of the thickness from the inner radius (bend radius)
Another method of specifying the neutral factor is to use PZL (Plastic Zone Legth) formulars from the material form
I personally like the DIN.PZL with the old DIN formular for steel sheet metals which does a good sheet job for me now since nearly 20 years.
If You want to enter bend area valueas regarding to radius and thickness YOu can use the ISOtable.PZL.
Be aware that YOu first have to register them from Solid Edge\custom\sheet metal directory (see help too)
Hope this helps.
PS.: a final personal opion here is, taht I don't like to use the Gage Tables.xls method.
This IMHO speeds down the performance for sheet metal operations, even it is the most flexible way to define values.
adding to the other. you can also switch to the "use excel gage table" method.
this gives a FAB shop much more specfic control based on real in house results...
you can set different properties based on material and gage.
but will the use of the Excel gage table not be a performance killer?
At least this is what I have in mind from the past and regarding to many posts in different Solid Edge forums
Thaks for the fast reply,
We already use the gagetable for complexe part with different radius and yes it is a performance killer (maybe the next thing I'll try to fix). I might have been unclear about what I have but in so far.
I am not able to put intext image as my computer freeze... find in attachement my variable table.
Now, in blue you got a series of test to check what should be the neutral factor. It all depends on the sheet thickness and bend radius. In yellow is the neutral factor itself. It is driven by the test in blue. In red is my problem. I am looking for a way to make the bend radius update itself depending on the client 3D files. I dont want to input it by hand for all files. The only place I know where to get the radius is into the bend table. So I am trying to pull the variable from the bend table to the variable table. This should update the bend radius as soon as I perform a "transform" feature into the 3D model. If the radius update, the neutral factor will also update as the test in the variable table will output something.
It get kinda confusing as I am uncertain of what I look for.
Basically, I am looking the pull the ACTUAL bend radius from a 3D model. The only thing I got now is the minimum bend radius.
Let me know if you need to know something else as I will be at my desk all day.
You need to do a few things.
First off, the inside radius IS the bend radius. for sheet metal calculations.
The radius of the neutral axis is R+T*K
Look up the basic sheet metal formula for Bend allowance and bend deduction.
You can set up variables to calulate the bend allowance and bend decuctions exactly as SE does for the sheet metal parts. You can even change the SE does the bend calcs by entering your own formula.
I attached a spreadsheet I set up for myself to look at bending numbers. Perhaps it will help.
A magazine called "the fabricator" has a running artical on sheet metal that is a great referance
What I've done in the past, is first create a template to import my step files. I take my .psm template, and copy & rename it IMPORT.par, and that is what I pick when I import a step file.
Now I can set my material and gauge to our shop standards already established in our material table.
Then, I Transform to sheetmetal (Tools, transform). Once I have done that, then I can pick Bend Radius from the Modify area, and here it shows me the radius of the model, and I can change it if I wish. NOTE: at this point, when you select Bend Radius, you can pick each bend and change the radius at the same time.
Maybe this is a different approach for your imported step files, it worked great for a project we did that had hundreds of files to bring in.
Thanks for that input.
I might have to change strategy. I like your way of doing it.
I might as well check for VisulBasic AutoBend feature. I was told that we use that in the past and it was great in time respond but was poorly made. There was some grey area where it would output a neutral factor of zero. As concerning as it get, DXF file were sent to the laser and productions were scraped. How bad was it? They told me that, at the time (7 years ago) the solution was to either enter the neutral factor by hand or to use the gage table...
Now, anyway I will take, I kinda have to test extrem limits as I dont want this thing to fail. I would like to have advise on how everyone does it as I am new to SolidEdge (but I can do some variable programing), to sheet metal and to my shop. I would like to save time with whatever I can. I believe that there is nobody that have the time or want to get theire hands dirty on the optimisation of this as its been 7 years that it is on the "to-do" list.
Correct me if I am wrong but and hour to get a STEP file to draft and DXF file is kinda too long for me. I believe it should be faster.
Anyway, I will take the week-end to think about all that and maybe find something.