Formed features in Sheet Metal environment

bryan_lagrange

Working in a sheet metal job shop we sometimes have formed features such as louvers that are placed on sheet metal parts that we manufacture.

When manufacturing sheet metal parts it is good to know how these features are added in the manufacturing process and what is needed from the CAD side to produce this.

The most common formed feature we apply are louvers, so I will use this as an example. 

To create a sheet metal part with louvers we use a CNC laser to cut the part and a CNC press brake to put the louver in the cut part (along with making bends). For the laser on the CAM side I need to have a line in the .dxf that will be used to make a kerf width cut to place the louver. The cut relieves the open area that the louver will make in the metal. When forming it I need to show location of the louver and type for the press brake operator (we have 2 sizes 5in and 9in long louver).

Here is how I accomplish it in Onshape (I will use my public account so everyone can have access to the Onshape document https://cad.onshape.com/documents/e527e3d9c840215a5e5ebef3/w/993910e9201c1d24fa058359/e/a0c7643ecc54f55ca7307515 ) :

First I created a library with the 5in and 9in long louver. I made just a surface of this feature so that when I add it to my sheet metal part, as a derived component, I can combine the surface and the part using the thickening command entering the thickness of the sheet metal part:

5in louver

I create my sheet metal part with all the features that will be needed to laser cut. For the louvers, I place a line then use the symmetrical offset with a.001" diameter. I will use this to make a cut into the sheet metal. The CAM software we use will recognize a .001" diameter slot as a single line, which is what we need to make the kerf width cut for the louver. 

I create a sketch of the cut, Remove extrude the sketch, pattern the remove extrude. I also place a mate connector where I want to place the derived formed feature on the part.

Since these are all the features I need to laser cut this part, I will finish the sheet metal part and get the flat pattern I need to create a .dxf (programmed in CAM) for laser cutting.



DXF of sheet metal part.



Now to depict the louvers onto the part. The depiction of the louvers in the manufacturing drawing is need for the press brake operator to place them and for final QC inspection:

I will use the derived function and go to my sheet metal formed feature library and select the louver I want.



I will use the transform command to place the feature via the mate connector.



I will then pattern the surface to the amount of louvers I need

I will Thicken and use the Add option to add the feature to the sheet metal part. In the thicken command I will enter the thickness of the sheet metal part.



For a final look I find using the move face feature helpful. I simply select the faces in the louver area that needs to be removed and move them to create a louver opening. This is an optional step if you want to complete the look. You could also use the extrude remove option.



Here is the resulting manufacturing drawing that both the press brake operator and laser operator (along with the .dxf file for CAM purposes) would use to create the part.

eric_pesty

We've come up with a very similar process with our louvers, although since we don't do the manufacturing ourselves, we use a solid for the louver shape instead of a surface and use a boolean subtract to create a louver outline in the sheet metal part instead of the line you use for your laser cutting (the sheet metal shop starts from the 3D model anyway rather than the flat pattern to setup the sheet metal parameters anyway). In a flat view on a drawing it's basically the same as if the louver was displayed in the flattened state (like SW does...).

We also use a single louver body with configurations for the different sizes we use instead of using separate ones, which makes it very easy to change to a different size louver if needed.

matthew_stacy

@bryan_lagrange, what is the threshold value of slot width at which a single kerf-width cut becomes a perimeter cut?  Is that default threshold width adjustable?

MichaelPascoe

Nice, thanks for sharing! It's neat to see other peoples work flows.

bryan_lagrange

I typed the width wrong on my workflow.  @matthew_stacy for the CAM software we use, If I make an oblong with a width of .000001 this makes the elements small enough that the CAM software reads the .dxf entity as a single line for processing. I am sure this would vary from software to software. You can change the oblong size by editing the sketch to what you require. 

bryan_lagrange

I also added the louver with an adjustable width in configurations.

bryan_lagrange

Now if we can get some cloud integrated 2D cutting (laser, water jet, plasma) CAM to go with Onshape. 

MichaelPascoe

@bryan_lagrange, this would be a perfect application for a custom feature. Do you do these often?

bryan_lagrange

@MichaelPascoe we do these fairly often on electrical panels. There are feature scripts to create formed sheet metal features already. Since we produce the parts, I need to produce a .dxf file for our CAM software that contains the geometry to produce the formed features. In the case of the louvers I need to have a single line laser slit in the flat pattern .dxf file. 

Formed features on sheet metal parts are probably more efficiently made using a CNC turret punch. On these machines you can do a variety of formed features such as single hit louvers, progressive louvers, dimples, specialty stamps, and host of other variety features. Depending on the CAM software, some would just need a start and stop point or a center point like a cross hair on the flat pattern to indicate where to place the formed feature. 

EvanReese

ooh! yeah this would be a great candidate for custom features. I'd picture something like a suite of features. Feature 1 could be used to set attributes on each library part (the louver model), which would store information about it, like how long it is. Feature 2 would take points or mate connectors as inputs, plus a part selected from the library, then it would create the lines and do the offsetting and cutting, as well as set attributes on the faces of the cuts for the next feature to read. Feature 3 would just take the entire sheet metal part as an input. It would need a finished sheet metal model or it could finish it for you. It would find all of the faces made by feature 1 (via face attributes), and do all of the work to actually model the 3D louver. It could pretty much be a 1 click feature. I don't do enough sheet metal to want to build this, but it could certainly be done.

Carlos_Martinez_Gonzalez

I use this Feature Script from Morgan Bartlett and am building my own forming tool library. It doesn't create the exact geometry on the flat pattern but a small cut that is enough for us to set the tool on the right position on the machining software. 

Fs: https://cad.onshape.com/documents/a752e0db24eb071ebb6f5aa0/v/b183b414b4b032149272ccee/e/e5c2abf7dd42d71d28468eca

Example: https://cad.onshape.com/documents/a10a02b6cd4e0f7135ebd75a/w/1eea426fd389eef3dff978e9/e/efac18eae0173ec1830b587b?renderMode=0&rightPanel=sheetMetalPanel&uiState=628c743009d1b23dcdd13f31

MichaelPascoe

Legit!