notching tubes in solidworks

[jesusgatos]

Wondering how you guys are notching tubes in SolidWorks when you want to show the tubes trimmed-back to full wall thickness. When working with flat sheetmetal parts, usually just cut through the part where it will mate with another part, and then convert any edges that need to be trimmed back from one side of the part to the other and use those to create new cut lines. Never really worried about it with tubes because I was always working with holesaw-type notchers, so didn't need to model the trimmed tubes. But what's the best way to do that? Don't see any options in the Weldment feature dialogue box, and creating a profile to sweep around the lines at the end of each tube manually seems really tedious. Any suggestions?

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[CRAIG_HALL]

I don't work with solidworks at all only soldedge. But I did see a works video showing a tube converted to sheetmetal and it trimmed all the edges to normal with the surface.

[jesusgatos]

Oh, that's interesting. Thanks Craig, I'll have to look into that.

[PDANK Racing]

[QUOTE=jesusgatos;1388693When working with flat sheetmetal parts, usually just cut through the part where it will mate with another part, and then convert any edges that need to be trimmed back from one side of the part to the other and use those to create new cut lines. [/QUOTE]
Can you explain how to do this? thanks

[jesusgatos]

Sure, I can try. There are a lot of different ways to do things in SolidWorks, and in a lot of cases, simply converting it to a sheetmetal part will trim-up a part pretty nicely. Had never occurred to me to try it with a tube though! Anyway, here are a few screen captures to show you how to do something like this manually. The example is just a motorcycle mount for an 8" racelight that I've been working on. See how the tab is oriented, relative to the tubes? How it's 'twisted'?







Started by inserting a new part into the assembly- and did all of the modeling within the assembly - so I was able to use other parts in the assembly to define the geometry for these mounting tabs. But there are some things about designing parts within the context of an assembly that are kinda screwy, and if anything changes, it's not unusual to see a whole FeatureManager Design Tree turn into a long list of red X's. One thing I've found that really helps with that is to use the 'Pack and Go' feature to save copies of all files within an assembly together in one place. Creates a lot of redundant files, but helps to maintain those 'external references', which it's important to note - must be turned on if you want to do something like this within an assembly. If you're only working on an individual part, you can disregard all this.





Created a custom sketch plane, then inserted a 2D sketch and defined the basic geometry for the part (was really only concerned about the location and the material thickness). Made the part oversized, intending to trim it down to size. Can see in this screen capture above how I used two different types of extrude features. The 1st extrude feature I used was 'up to surface', and I selected the tube that I wanted the tab to hit. The 2nd extrude feature (going the opposite direction) is a 'blind extrude', which I did because the way the tab intersected the bottom tube, it didn't allow the 'up to surface' extrude to work properly.





Notice how the tab is already trimmed to fit the upper tube? The 'blind extrude' required an extra step, which was to manually trim the tab where it intersected the lower tube. Did that by creating another custom sketch plane, inserting a 2D sketch, converting the tube profile geometry, then using the extrude-cut feature to trim the tab to fit the bottom tube.







Now we're finally getting to the part that you were asking about. Can you see how the tab wraps around the tubes? All you have to do is insert a new sketch on one face of the tab and use the convert tool to transfer the edges of the tab from one side to the other. Then trim/extend those and do whatever else you need to do to create a cut path, and use the extrude-cut feature to remove that extra material, leaving you with a part that fits the other parts, and has been trimmed to create a shape that you can cut.

Hope this is helpful. Just ask if you have any more specific questions. Like I said, there are a lot of different ways to do things, and there are many people on here that know a lot more than me. Maybe some of them will give you some other good suggestions. Know that I've received a lot of help from a few people on here with SW-related questions over the years.

[PDANK Racing]

Thank you for the detailed instructions. I'm a SW noob, right now the only thing I can draw easily are dimple dies. I think I have a grasp of what you explained and hopefully will get some time tonight to try it out.

[jesusgatos]

I don't work with solidworks at all only soldedge. But I did see a works video showing a tube converted to sheetmetal and it trimmed all the edges to normal with the surface.

Can't seem to figure out how to convert tubes into sheetmetal parts. Tells me that I have to select a planar face, and then when I select the end-face of a tube, it wants to delete the rest of the tube, only maintaining the end-face profile. Related question: can parts can be weldments and sheetmetal parts simultaneously?

[StokedMotorSport]

the way ive seen it done. is to draw a small rectangle across tube face. .01 mm x length of tube cut through wall thickness and flatten part.

[jesusgatos]

Sorry, not sure I'm following you. Confused by the .01mm rectangle (wouldn't that create two separate bodies in most cases?) and the 'length of the tube' (aren't we only talking about the end-faces here?) and flattening the part (have only heard that term used when referring to sheetmetal parts).

[StokedMotorSport]