I just tried to do the same thing. not a chance, no way. no work around.
No matter what you do, I could not find a way to get text to display as result of math.
The gauge is not available for display in draft.
This is created a huge problem for me. I wish there was a solution.
I am just moving from Solid Edge. The relation between gauge and the BOM was the core of my drafting system. 90% of my parts are sheet metal.
The one work around that failed for me was what a call a singular filter. With very complex logic, all parts in a thickness rang can be displayed as a specific value. But as soon as you have multiple materials or radius, or neutral factors for a single thickness range, it does not work.
From my perspective on Solid works, this is bug/problem #1
just thinking out loud, I think this may be achievable with Property Tab builder.
if you have the tooling information and the Gauge table information in the same spreadsheet.
I'll play with it tomorrow, do you have a screenshot of what you want it to look like?
Chad Hawkenson - The only way I would see it working is to set up a "Sheet Metal Part Template" with a design table and have the equations in the design table reading the dimensions and then returning those values through your formula. The only issue with using Design Tables is that if and when you make any changes you will need to edit the design table to make sure that it is properly rebuilt..
These already are, or can be, properties in the part file.
Material is always there and not tied to sheet metal (or anything else).
Gauge (in the part's units) is the Thickness global variable and the bend radius can be taken from the radius of any bend feature (assuming it doesn't change from bend to bend, but if you're looking for a single then I'm guessing it doesn't).
The tooling can be added as a custom property to the part as can "Dev. Of 0 Per Each Bend" (whatever this means).
All of these can be referenced in a drawing note, either separately or together.
Perhaps you already know this, but by having a flat pattern view (which can be outboard of the sheet if you don't want to see it), you can
add this dynamic note (right-click the flat pattern view, select Annotations>Cut List Properties w/an updated cut list):
Both the OP and myself want the single most important piece of information about the sheet metal. What Gauge it is. The thickness is not gauge. How do we handle say expanded metal, or diamond plate, or aluminum vs carbon, etc. displaying the gauge is the right way.
This might not be what you are looking for but we use a macro to determine gauge and square feet. The part needs to be flat (flat pattern or just a flat part). You will need to set up different ones for each material type and then edit the macro with your desired information but this might get you started.
I am attaching the macro for you to see.
Area Tesselation.swp.zip 38.9 KB
The current work around is that we have to both select a gauge and material. There is a material for every gauge. But this allows for much larger chance of an error by the operator. The goal is to have all the material details handled by a single switch (Gauge). Then there is less chances of mistakes.
Details: Material, Thickness, Radius, Neutral factor, Visual representations (Both 3D and 2D), Weight (Expanded metal / Diamond plate get tricky)
As Mr. Stoltzfus mentioned, you can use a design table and leverage Excel to generate what you need into custom property columns.
Attached here are the same files I attached at the bottom of: Sheet metal Gauge
It uses lookup functions, based on the gv Thickness, to look up the gauge, which then populates a custom property cell.
The material is read which looks up a k-factor and if the material isn't specified then a red note displays such on the drawing.
Perhaps you can use this file as a basis for what you're looking to accomplish.
Repeating Mr. Stolzfus, you will need to maintain the DT for new materials, changes, etc, but with the DT as part of a sheet metal part template, changes should be fairly easy unless they cascade heavily into existing part files.
If possible, I'd trim the list to the gauges and materials you'll encounter.
Once established and running, perhaps DT changes won't be too often.
I hope it helps.
Thanks Kevin, I am going to look through this.
This is the actual spread sheet I have created for figuring if a supplied flat pattern will work with our breaks/tooling. As I change the Material type (Mild Steel/Stainless), Thickness (Via a table lookup), and available bend radius base on thickness (via a vlookup) I can then pull the tooling information from a table as you see in the bottom right high lighted line. It will string together the material information, bend radius, tooling required and deviation from calculated flat to supplied flat and take into consideration called out tolerance. It will actually flip Go or No Go based on user inputs.
My question can I get S.W. to do the same thing and push it to a custom property that I can have in the drawings I produce? From what I can tell all the information is right there from the Gauge tables I have set up, there is just no way to get that information out and append a small detail of information like Tooling that would correspond directly to the selected material.
I appreciate everyone's input on this.
You just hit the nail on the head. The Gauge can't be displayed in draft and the material can't be driven from the gauge. If they would solve those two details, that solves everything, if all the information can be used both piece by piece and for parts lists.
We have worked very hard on developing a macro that delivers this (seemingly basic) information.
The macro calls on the cut list information; converts it and applies it to the custom properties where we can then have those dimensions automatically input into our templates and BOMs.
I did not write this macro, but I wanted to comment that it is possible.
Cut List Info:
I'm experimenting with the Custom Property Tab Builder (CPTB) right now, and I think that you could show gauge with this method.
(Side Note: The way I am currently testing would involve moving away from the gauge table.)
It is in the early stages of testing, and might be a little convoluted, but this is what I am playing around with . . .
We have a spreadsheet with reference information for our bending, so I am using the List Group within CPTB to make my selections and create custom properties based on the spreadsheet.
The "Material" pull down has our common sheet materials.
The "Thickness" pull down has the thicknesses available for the material chosen.
The "Bend Radius" pull down has the available tooling for the material of that specific thickness.
The "K-Factor" and "Bend Deduction" are based on all of the information above.
(Usually these only have a single option in the pull down menu, but some of them will have multiple, depending on the specific dies used.)
All of this is populated from the spreadsheet mentioned above.
I have a part template for sheet metal that is linked to these values.
This allows me to start a new part, open the custom properties tab, populate all of the information above, sketch the profile, create my base flange, rebuild, and all of the information is pushed to the part.
Any changes can be made through the custom properties tab.
All of these items are now custom properties that can be used wherever needed.
If you were to add a column that shows Gauge to the spreadsheet that is used for the List Group, you could add that as a custom property.
I'm not sold on this idea yet, like I said, it is just an experiment right now - there are things I like, things I don't like, but maybe it will give you some ideas.
I do like how the list group "funnels" you toward the necessary end result - in this case it is the K-Factor or Bend Deduction.
- It also prevents you from getting a thickness that is not available for a certain material, or picking a bend radius that won't work.
(I am testing something similar for powder coat colors - giving a bunch of different ways to get to the final powder part number.)
Very early stages of testing, we'll see what happens after I put it through the paces a little bit more.
I may end up going a completely different direction, who knows . . .
If you can get that to work, I would use it. We have the same set of problems and most of what I do is custom sheet metal.
Between myself and one other CAD person, we create about 10 new pieces of sheet metal a day on average.
That was the way I was thinking of going, mainly because I am poking around trying to learn CPTB right now.
Can you answer a question for me? Where do I set the tab SW is looking for? In the picture below I have 3 tabs in the file the custom properties tab is looking for. However not the tab it is looking for. As you can see the button at the bottom is greyed out. That was where I expected to change it.
Andreas Rhomberg wrote:
Jim Steinmeyer , it is set in the file location settings for Custom Properties
Unfortunately, I have already done that. The part was originally designed by another user who has his own personal copy of the property tab in his own separate folder, something we see way too much of here. I have created a new property tab with additional features and would like to point the part to that tab instead of the other user's while I get it ready for the company standard. I have the folder set to the correct location unfortunately it is still looking for the other tab and I am unable to select a different tab name. I should be able to do that with the button at the bottom of the menu but it is greyed out and inaccessible. Selecting a differently names tab is where i am having my problem. There are 3 different prtprp tabs in the folder is is looking into and I am unable to access any of them instead of the original one.
Thank you. That was it. I was focused on the button on bottom and didn't look at the bar on top.