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Modeling in SolidWorks is pretty dang easy. Sure there’s little bits of wisdom that come with using it, but an installation and a day later and you’re on your way. The sheet metal features in SolidWorks are a little different. There more like trying to do a back flip. It looks easy, I can picture myself doing it, but I try and land on my neck. That’s what happened when I first started trying to bend things this way and that.
I would say 72.3% of people doing sheet metal design haven’t been trained.
The first time I took a Sheet Metal Training Course, I was the one teaching it. I learned a lot about what I didn’t know. Once you know some stuff thought, and like a back flip, designing sheet metal stuff can actually be kind of enjoyable. The kind of stuff you want to show off to your friends. Here’s a few items to get you on your way.
Step 1: Get a Mat and Learn about it
Whether its a training course or sitting down with Freddie Break Press from the shop, learn some things about sheet metal design and using it in SolidWorks. The best thing you can do is talk with someone that has been doing it a while in your company. Someone that knows the tricks to make it work. They usually like Philly Cheese Steak sandwiches for some reason.
Get manufacturing information from the shop
The guys and gals that make the parts can tell you a lot. Make it a point to spend some time with manufacturing. Here’s a short list of items you will want to ask about.
How do you use a drawing received from engineering?
- What bend tools do you have?
- Do you have a bend allowance table?
- Do you have a stock list?
- What is the lead time on getting materials?
- Do you use CNC equipment?
- What formats do you use?
- How do you import 3D geometry?
- What information do you need/lack from the drawing?
Use a solid to control the sheet metal
It’s kind of like using sketches to drive a design but I would liken it more to a form that you build around.This is really useful because it keeps all the feature definition in one spot and can help line up important features between parts. It’s also useful to see how your bend radii could cause interference.
Create half a part and mirror
This is probably the first thing I learned about sheet metal that saved me a lot of time and headache. I would construct the model like it was cut in half and create the symmetrical features. Then I would mirror it and add any additional asymmetric features… then realize they needed to be symmetric.
Use color to separate parts
Color can help avoid a lot of mistakes. Instead of having a bunch of gray slabs of 2024-T3, add some color to the individual parts so the interaction between each part is clear. If you use shaded views on drawings or your manufacturing uses eDrawings or color PDFs this can help them tell the pieces apart.
Create your own set of forming tools
SolidWorks comes with some examples of forming tools. You can add these to your Design Library in the Task Pane on the right side of the screen by going to Options, selecting File locations and Design Library from the pulldown and going to
Create a library of flat patterns
Commonality among sheet metal parts is a great asset. You won’t always have similar parts but if you have a nice library, you’ll find it easier to start or give someone to go by. Storing them by flat patterns can make it quicker to find because you become familiar with the shape after working on it. After you develop a nice library and find some re-usable pieces, make some templates to speed up your design.
Line up features using equations
You need a tab to line up with a slot. Instead of changing each dimension every time you need to make an adjustment, link the dimensions together (select two dimensions, right-click, link values) or set up some equations. The design may be finished by the time you’ve done all the tweaks and realize you could link them. Go ahead and do it so it set up for the next time.
Teach your methods to the company
Time to give away your secrets. One of the biggest problems I see people have with making sheet metal parts is not being taught how to use it. While it’s similar to making regular parts, there’s thing you learn after being familiar with the product you’re making. Showing someone else how to do an unbend-cut-chamfer-bend operation to get a better outcome will save time and eliminate frustration.
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What I desperately need is a way to extract the
sheet metal size of the flat pattern. There is no information provided by solidworks except that I know solidworks must have a X@flatpatern, Y@flatpatern, & Z@flatpatern.
(Thickness, Width, Length)
Otherwise, the geometry could not exists.
QUESTION: What are the three (x,y,z) variables are?
or
Is there a macro to obtain these values & add to properties
For Thickness;
Go to File > Properties > Custom tab
Under Property Name type ‘Sheet Thickness’ or similar.
Click in the Value column and select ‘thickness’.
The Value column should now show your sheet thickness.
The value can now be linked into your drawing notes etc.
Hope this helps.
Thanks Alex. Custom Properties are definitely the way to go. Great to use as a check also.
Thanks for you tip. However, I need more than Thickness.
I also need length & width. What I am trying to do is create a somewhat
automated cut list for thousands of sheet metal parts used in a large
assembly. With help of “ToolWorks” (a third party SolidWorks Partner),
I can genarate a Top level BOM. From Assy. Model. ToolWorks also has the ability to automaticaly extract values from d1@sketch1, d2@sketch2, etc.
Since SolidWorks already knows the size of the flat patter, I was looking
for x1@flat-patern1, y2@flat-patern1, z1@flat-patern1 and extract
these values via VB macro. (provideing model variables even exits)
I don’t know. .. but it looks like NOT!!
Failing that, I’m stuck having to go back to a couple of thousnad parts
and measuring the flat patern. What shit when I know SW already calculated
the sizes but can’t get at them.
This makes sheet metal functions very poor in SW a way too maual.
Ernest -
If you go to the Kansas City SolidWorks User Group website (kcswug.com), Wayne put his Most Excellent SWW2007 Sheetmetal Presentation in a zip file you can download. On page 107 of that presentation (did I mention how excellent it was?) there is a description of a method to extract flat pattern dimensions. I know it’s not “automatic,” but it is parametric, so there is certainly value in that.
Thanks Steve, here is the direct link to the site and that zip file (13.4 MB)
Many Thanks to Steve R. & Josh …
Have downloaded zip & have a look.
Thank you both for your help.
Ernest
Interesting problem for you….
I have two configurations of a sheet metal part, but i want to use a different thickness for each configuration. That in itself is not the problem - this is easily done by double clicking the part and changing the linked value - but what doesn’t change is the bend allowance/deduction. is there a way in which i can change this too?
Hi Ed, you can do this fairly easy with a Gauge Tables and Bend Tables. There’s sample ones in C:\Program Files\SolidWorks\lang\english\Sheet Metal Gauge Tables and \Sheetmetal Bend Tables. You can take one of those and modify it to what your shop uses. To use these, In the Sheet Metal Properties, select the gauge table in the Sheet Metal Parameters, and select Bend Table in the Bend Allowance pulldown. Your shop may have these values set up already, so check with them first.
Hi There,
We are a Indian based company. We have developed a software based on SolidWorks for Sheet Metal. It generates Cutting & Bending drawings for Sheet Metal parts with all information required for costing of Sheet Metal like thickness, no. of pierces, cutting length, no. of bends & surface area etc.
Please let me know you no. so that I can explain you this further.
With regards,
Swapnil.
I have been able to extract flat pattern sizes by flattening the part and drawing a box around the edges and making them construction lines. Set all lines colinear with each edge and dimension them and set them as driven. set each dimension on to “Length” and the other to “Width” this will allow you to read the length and width of the flat pattern. Make sure to call the sketch “cutsize” under configuration specific properties creat a value called ie: “Length@cutsize@@Default@Part1″ and do the same for “Width”
You will have have to use a Macro to fold and unfold each configuration. Here is the Macro is use to unfold and fold all configurations: remember you have do run this macro to be able to update all configurations with thier appropriate flat pattern dimension.
Dim swApp As Object
Dim Part As Object
Dim SelMgr As Object
Dim boolstatus As Boolean
Dim V As Variant
Dim i As Long
Dim retval
Sub main()
Set swApp = CreateObject(”SldWorks.Application”)
Set Part = swApp.ActiveDoc
Set SelMgr = Part.SelectionManager
retval = Part.GetPathName
boolstatus = Part.Extension.SelectByID2(”Flat-Pattern1″, “BODYFEATURE”, 0, 0, 0, False, 0, Nothing, 0)
Part.EditUnsuppress
Part.ClearSelection2 True
boolstatus = Part.Extension.SelectByID2(”Flat-Pattern1″, “BODYFEATURE”, 0, 0, 0, False, 0, Nothing, 0)
Part.EditSuppress
Part.ClearSelection2 True
V = swApp.GetConfigurationNames(retval) ’since Part = swApp.ActiveDoc; otherwise should be path & filename of doc
For i = 0 To UBound(V) ‘loop for each config name set to variable i
boolstatus = Part.Extension.SelectByID2(V(i), “CONFIGURATIONS”, 0, 0, 0, False, 0, Nothing, 0)
Part.ShowConfiguration V(i)
boolstatus = Part.Extension.SelectByID2(”Flat-Pattern1″, “BODYFEATURE”, 0, 0, 0, False, 0, Nothing, 0)
Part.EditUnsuppress
Part.ClearSelection2 True
boolstatus = Part.Extension.SelectByID2(”Flat-Pattern1″, “BODYFEATURE”, 0, 0, 0, False, 0, Nothing, 0)
Part.EditSuppress
Part.ClearSelection2 True
Next i
End Sub