Sheet Metal - Custom Properties
Sheet Metal - Custom Properties
(OP)
We use only 3/4 different thicknesses of sheet metal to make cabinets etc. I am wondering is it possible to assign custom properties to a sheet metal part as defined by its thickness. For example, it would be ideal if whenever one of our engineers began building a cabinet in 3mm sheet that solidworks could recognise that 3mm sheet has a Part Number XXXX. Other properties I'd like to add are sheet size, Supplier etc etc. My end goal is to have a BOM on the assembly drawing listing the part number of the sheet used, the weight used and maybe supplier. Is there any easy way to do this without having to manually imput each time I start a new part?






RE: Sheet Metal - Custom Properties
We do this for injection molded parts, sheet metal parts, die cast parts, machined parts, etc.
RE: Sheet Metal - Custom Properties
RE: Sheet Metal - Custom Properties
Rob Rodriguez CSWP
www.robrodriguez.com
SW 2006 SP 2.0EV
RE: Sheet Metal - Custom Properties
It sounds a little complicated but it does seem to work.
RE: Sheet Metal - Custom Properties
Jason
UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2
RE: Sheet Metal - Custom Properties
any thoughts on how to accomplish the same thing for parts with more than one dimension defining their raw material such as flat bar defined by width & thickness, angle defined by two legs & a thickness, etc. then i could have a flat bar template, angle template, so on to go with my newly designed sheet metal part template.
RE: Sheet Metal - Custom Properties
To populate your Folders simply open a new part. Click a plane and start a sketch on the plane. The sketch will be the cross section of your flat for example. Add lots of points to your cross section (for example in the center of the flat as wells as at the midpoint of all the lines in it). Exit the sketch. Now using a design table or indeed simply using the File-Properties menu you can assign custom properties to this profile such as part number, Material etc. Now simply click once on the sketch in the feature manager Design tree and go to file save as. Select file type as being Library part and save the file in the appropriate weldment folder as created above. The great thing is that the weldment profile saves the custom properties too. Now everytime you design a flat you will have the part number and material. The weldment drawings can then have a cut list which you can customise to show your custom properties. One other hint. When you draw a part using weldments you must 'update' the cut list so that it appears in the cutlist table in the drawing. Just right click on the cutlist icon in the feature manager window and select update. Finally, if you are not familiar with weldments then have a look through the help files - they are pretty decent.
RE: Sheet Metal - Custom Properties
RE: Sheet Metal - Custom Properties
RE: Sheet Metal - Custom Properties
RE: Sheet Metal - Custom Properties
I have been using the design table approach to read in plate thickness and populate raw material p/n, description, etc. i seem to be having good success doing things this way.
I also figured out a way to do the same for multiple flat bar raw material sizes. i start with a cross section of the flat bar i.e. 1/2x2. 1/2 is named thickness@sketch1, 2 is named xdim@sketch1. i concatenate these two values to come up with a value unique to only one size of flat bar from our database. my example would produce (0.5 2) I have also created a spreadsheet with all of our flat bar sizes concatenated (suprisingly that didn't take too long to build). I then apply the same vlookup method from my sheet metal table to read raw material p/n, description, etc. of our flat bar database. (hopefully that last paragraph made some sort of sense). i haven't gotten this far, but i don't see why this method wouldn't work for angle iron, channel, etc. leaving me with a part template for each form of raw material.
**now for the questions.
1) is there a way to have my values populate the custom properties tab instead of the configuration tab?
2) is there a way to automatically update the design table? currently if i change sheet thickness, i have to right click-edit table for the values to "refresh"
RE: Sheet Metal - Custom Properties
The only way to update the design table is to open and close it. You could probably create a vb macro that will do it. This site has something to get you started: ht
Jason
UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP3.0 on WinXP SP2
RE: Sheet Metal - Custom Properties