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?
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Sheet Metal - Custom Properties 2
- Thread starter neilc78
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- #3
I was thinking of doing that too. Problem is that we design many parts in context within the assembly. When you do this the 'default template' as defined in document properties is always used when inserting a new part. This means that you must change the default everytime you insert a new part so that the correct thickness template is used. That is a bit of a pain. Even worse, what happens if you decide mid design that the part thickness of 2mm you started with isn't strong enough and you want to change the thickness to 3mm? To me it looks like any template part would need to cover all available sheet thicknesses. I haven't got my head around how to do this yet!
There is a setting in Tools/Options under Default Templates named "prompt user for document templates". This will allow you to select wich template SW should use when you are creating a part in context of an assembly. It works very well.
Rob Rodriguez CSWP
SW 2006 SP 2.0EV
Rob Rodriguez CSWP
SW 2006 SP 2.0EV
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- #5
Thanks for the help. The problem with using a template for each thickness is that you can't change thickness mid design without losing all the information you assigned to each template. Here is what I am working on doing. I have noticed that when you begin a sheet metal part the first dimension defined is always the thickness, this will be called 'thickness@sheet-metal1' (as long as you don't rename sheet-metal1 feature). I began by drawing a simple sheet metal plate of any thickness. I then insert a design table (allowing changes to be made from the model). In the design table I enter the 'thickness@sheet-metal1' variable. A few rows below I have some more cells. There will be a list of thicknesses and opposite it them in the same rows will be the associated properties such as Part Number etc. Back up on the top row I add some custom properties using $prp@partnumber. To define this I ask excel to use the thickness recorded as the 'thickness@sheet-metal1' variable and use the vlookup excel function to search my table of cells below to find the appropriate part number. On exiting the design table I delete the base flange feature and save the part as a template. Now when I start a new part and define a thickness at the first base flange, this will automatically populate the design table and the table will search for the appropriate custom properties for that thickness.
It sounds a little complicated but it does seem to work.
It sounds a little complicated but it does seem to work.
jobiewan99
Mechanical
neil- i can't express how happy i am that i stumbled across your solution to this issue. i have been trying to find a reasonable solution to this problem for quite some time.
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.
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.
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- #8
No Problem, I'm glad you found it useful. The good news is that the solution to the 2nd part of your question is even easier. I achieved that by using weldments. The standard weldments to not include flat bar and I'm sure that the cross sections covered within Solidworks don't cover all the Angle, Box etc that you use either. Weldments profiles are all located in the folder Program Files/Solidworks/data/Weldment Profiles. There is nothing to stop you adding new folders in here to cover your weldment types such as flat and Angle.
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.
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.
jobiewan99
Mechanical
i guess i was hoping to create more of a "one stop shop" as in a flat bar part template that would have some sort of formula that said if width equals 2 and thickness equals 1/2 then it would return part number description, etc for 1/2x2 flat bar. then you could just open that part define the flat bar dims and extrude and you would be finished. the draw back to what you described is that i would have to sit down and create profiles and populate custom properties for hundreds and hundreds of sizes of flat bar, angle, etc.
- Thread starter
- #10
It could take time all right but Drawing frames and the like using weldments is so much faster than extrusions and cuts that that time would be made up. You could try doing something like what I said before but you would have to make sure all your designers are disciplined enough to call the length x width dims l and b each time (or alternative) then you could incorporate that into a design table. My guess is that it would get too messy. I'd give serious consideration to weldments if I was you.
jobiewan99
Mechanical
yeah, the biggest roadblock i came across was trying to develop the equation/formula that would be able to decipher my table with 100+ sizes of flat bar and having to test two variables (width & thickness) as opposed to one
jobiewan99
Mechanical
2 months later......
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"
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"
You would have to write some VB code inside the excel design table to populate "Custom" Properties instead of "Config Custom" properties. I have a design table that does this, it enters "Revision", Part family prefix, and part family prefix description into the regular custom properties via VB. Then in the design table, I concantenate these prefixes with the rest of the description for each config to get a full config description and part number.
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:
Jason
UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP3.0 on WinXP SP2
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:
Jason
UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP3.0 on WinXP SP2
- Thread starter
- #14
I believe that Gildashard is correct in both cases. I have put the open close of design table on the long finger for the moment but at some point in the future I intend to write a VB macro that will open each part in my assembly and then open and close the design table in each part in order to refresh. At the moment there is no other way to do it.
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