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Real-world projects are vital to mastering SOLIDWORKS, and sheet metal enclosures are a perfect example of a typical project. Sheet metal enclosures house and protect circuitry, wiring, and other sensitive electronic parts and frequently require customization by a professional CAD designer. So take a firsthand walk through designing a sheet metal enclosure for circuit boards and panel-mounted connectors, as well as fans, power cords, and switches, with SOLIDWORKS. Gabriel Corbett covers the key techniques for working with in-context parts and assemblies that dynamically adjust based on the master part model. He'll show you how to use equations to drive the size of the box and calculate vent holes, work with circuit boards, and download connector components. Plus, learn how to add decals before prepping the final drawings for manufacturing.
In this movie, we're going to be saving out a DWG or DXF file. I have the 6.4-1 part drawing opened up, and I'm at the same point that I left off in the last movie. And we're ready to save out our DWG or DXF file at this point in time. I just want to go over a few of the options and things we can look at for doing so. Now, it's pretty simple once you've got this scaled 1 to 1. Before we do anything else, let's double check that we've got that. So right-click anywhere in the Drawing view.
Go to Properties, and make sure it does say 1 to 1 here, and we've got a sheet size that's reasonable for it to fit onto. Click OK and then again click on the item it self. And slide down and make sure you've got scale as usheet scale and make sure that sheet is 1 to 1. So, at that point in time we're good to go. I do also want to point out that we are referencing the 6.2 files here, but we're on the 6.4 drawingsheet. Okay. Now, at this point just go up to File > Save As and if it gives you this little warning you need to update the views, that's okay.
Go ahead and click on Yes. Now, as far as our save as format, by default it's trying to save it out as a SolidWorks drawing. But I don't want to save as SolidWorks, I want to click here and save as either DWG or DXF. So either one of these ones here. Really the options are just about the same. So, first I'll save a DWG, click on that and then click down here on options, and gives you a lot of options here so, first off is the version. Now you might be tempted to go to the very latest version; I would caution you away from doing that. The best one that I've found is the 2004 through 2006.
It gives a fairly small file type and it's pretty easy to open in a lot of different formats and a lot of different software will use that one. You can go all the way back to R12 and the further you go back. The more uniform it is, then almost any software will be able to open this file and use it. The further you go up to the latest version a lot of people are using older versions of the software and they won't be able to open the file. But a lot of times in the newer versions they'll be smaller file types when you finally save this thing out. Instead of being two megabytes it's a half a megabyte or something like that so you might just want to play around with.
Saving out several different versions and seeing which one works out best for you, but. Like I said, I recommend this 2004 through 2006 version. And then as far your fonts and things like that the AutoCAD one seems to work fine but you have a few different options here. And then down here you've got some enable scaling 1 to 1, so if you didn't click on those things, if you enable this, make sure you're scaling 1 to 1 which is kind of helpful. And then down here a couple other options, you've got exporting splines as splines or as poly lines.
So, if you export as a poly line it's going to take a spline, a complex curve, it's going to break it into small little line segments. I basically many lines to create the design and sometimes I'll end up with faceting on your design if you laser cutting it depending on your resolution settings, so I'd be careful about using that one. I prefer trying to export a spline as splines but if you do have some issues. With the software they're trying to import it with, you might try the poly lines option as a class b resort. And then same thing here is exporting, do you want to export all the drawing sheets or just the one I'm working on right now? In this case here, the only one that makes sense is the sheet I'm looking at.
Not all the other assembly drawings in other views, so I only want the active sheet, and I click on OK, and I'm going to save that as chapter 6, and I'm going to put it in 6.4 finished. Click on Save, and it saves it out. Now that's one way to do this, and doing it as a DXF is exactly the same, so click on File > Save As. Drop down here to DXF. And click in here. And we're going to save it as, 6.4 finished. And click on Save. Is it enabled? Yes, that's okay.
Okay. Great. We've saved out both the DXF and DWG files of this and we're ready to move forward. I do want to point out one of the things. We can do this without actually creating a drawing at all. Click on the part here, or go back one view. Here's the view in the fold state. Open that view up. Here it is. Now, notice the flat pattern is right here at the bottom of the screen. So if I go over to Sheet Metal, I can also go over here to Flatten. I can see the flat pattern. And it gives you a nice rectangle of the outside finished sheet of material you're going to use.
And if I right-click on this, I have the option of right here exporting to DWG or DXF right here at the bottom. So click on that and do a Save As or Save as Copy, which is great. So Save as Copy. Save it as a DXF file or DWG file. Again, let's go up to chapter 6, 6.4 finished. And we'll just leave this file name which is going to be Flat Pattern 6.2, but it's really going to be 6.4. So, we'll change that file name.
And, again, we click at the options. They're going to bring up the same options we just looked at. Click OK. Click on Save. And that's going to ask us what do I want to export? Do I want to export the sheet metal, the geometry? You can export all this information here. Which is pretty handy. I'm just going to use the basic stuff here. Click OK. And it should pop up with a little view of what's going to be exported. And there it is. So it's giving you the outside lines, all the interior data. It is giving us the back side view. Remember if we looked at the view before we had the.
Counter sink's on the other side, so we might want to flip that. But in this case here, I just want to point out that we can do this. And when you're happy with it, go ahead and click on Save. Save at your file, and we're ready to send these files now to a laser cutter or water jet cutter, and actually build the part.
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