All,
I created the attached part and wanted to create it out of sheetmetal. Looking for tips on how to get there.
The highlighted green radi, is where I am assuming the fab house is going to have to weld two pieces together to make my part.
Cheers,
Jack
2 pieces can be welded together or it can be done as 1 piece by stamping process
Christian,
Yes, I agree. We will not send part out for stamping, so it will go to our sheetmetal vendor. I would like to model it up in solidworks using the sheetmetal tool and then maybe the final is an assembly that has the two pieces fitted together showing the weld? Not sure how to do that.
Making the solid a shell was the approach I took but not liking the accuracy, especially the hole locations...
I don't think it's good practice of making a solid (with shell) for sheet metal
start with a flat sheet and bend it to the shape you want and use punch tools for all cut out
There is a Convert to Sheet Metal tool available that will take a model and make it sheet metal. In this case you'll need to change some things. Talk with your shop about how they would want to build this part. Then:
MIke,
Yes. I know and I have used the convert to Sheetmetal tool. Gives me a few gaps that management does not like to see.
In modeling the bottom piece in sheetmetal, I fold up the correct modified "U" shape and then cut a triangular shape at 15 degrees to get the correct slope I need for the cover piece. The result is a surface where you can not attach the top piece. When you flatten the "U" shaped piece you see that in creates a complex curve. Thats the portion I am stuck on for creating the part out of sheetmetal pieces.
J
Of course. The gaps you are talking about, are they bend reliefs? The complex curve you mention, is it a spline in the bend area? And your shop doesn't like the splines. That would make sense, here's how I get around those issues. Think about your model a little differently. Make a part that's bigger than the final piece, and then cut away what you don't need. This way you get around the automatic features and you have complete control over your model.
Starting your part in Sheet Metal, begin your base flange as a rectangle with the maximum part height. Construct your edge flanges to get the basic shape of your part. Then select the Unfold tool flatten everything. Now make a Cut-Extrude to achieve the profile you need. Finally Select the Fold tool and proceed as you need. Notice there is a difference between Fold / Unfold & Flatten. You use Fold and Unfold to create features in your tree that you can use to define your part. The Flatten feature allows you to view the flat pattern to generate your output (DXF) and create a flat drawing view.
Hi John
I've used the convert to sheet metal and a few delete face tools to get to the point of having two parts to weld together. please find the part attached.
Hope this helps!
Dave
David,
I did not see the attachment.
J
First your are going to want to suppress any holes and the green radi edges because these a counter sunk that needs to be done after the flat as a post process just like if you where to make it in real life. you can put regular holes in so that they can be cut on the laser then all that is needed after it comes out on the laser is the counter sink of the hole.
Because the model is already made this should be very easy. Also no punch is needed because it will be all laser cut.
We are going to use the convert to sheet metal tool to make this part. Make sure you have keep body checked and choose a flat face to start the command then we are going to need to pick the bends. You can't use collect all bends in this method you must pick manually.
After your done whit the command it should look like this.
it looks the same because we kept the body so now if we hide it it will look like this.
if we hit flatten we see we get the flat pattern.
Next we do convert Sheetmetal again to the top and this time turn off keep body and we have both sheet metal parts.
that should give a good start and a few tips let me know if you need more info to finish.
The less welding the better.
I'd bend everything except the 2 large radius corners.
Although you could bend those onto the sides.
Agree ! welding is expensive - should be minimized or avoid it !!!
I bet the sheet metal shop might need a jig (add co$t) to hold 2 pieces in place before welding
As Bob suggested, this should be one piece with few spot welding
John,,, you might want to take a look at this. It actually was quite easy. I used your geometry but first changed the outside fillet radius to something smaller in order to close the gaps for welding. For manufacturing purposes it does not matter what the radius is in the model. I usually use something really small like .010" or less. That does not effect your overall dimensions. I offset your surfaces (0), then thickened, then did an insert bends. I did suppress your c'snks prior to offsetting then used your holes wizard sketch points to place new c'snks in the new sheet metal. As a former brake operator (and everything else) this is a nice break from the mundane. Not too hard - not too easy.
I did this over your model so you can unhide yours and compare. Looks like the flat could be easily punched so you can get the c'snks in the turret also. Or they might want to do a punch laser combo.
Dennis,
You are quicker to the trigger. Exactly how I would build it. Great minds....
Exactly what I thought - No need a jig ($$$) for this approach
Dennis,
I'm on 2015 so your part came over as a future version which I can not see the steps or modify. The pictures you provided give some insight into how it's made. This was what I was envisioning doing but did not know how to get there.
Thanks,
John
John,,, you might want to take a look at this. It actually was quite easy. I used your geometry but first changed the outside fillet radius to something smaller in order to close the gaps for welding. For manufacturing purposes it does not matter what the radius is in the model. I usually use something really small like .010" or less. That does not effect your overall dimensions. I offset your surfaces (0), then thickened, then did an insert bends. I did suppress your c'snks prior to offsetting then used your holes wizard sketch points to place new c'snks in the new sheet metal. As a former brake operator (and everything else) this is a nice break from the mundane. Not too hard - not too easy.
I did this over your model so you can unhide yours and compare. Looks like the flat could be easily punched so you can get the c'snks in the turret also. Or they might want to do a punch laser combo.