Sheet Metal Patterns

[phatfred8]

Hello,

A friend asked me to try and get a offset cone drawn and then unfold it to have a templet for cutting the part out. I can do it the old fashsioned way(drafting and layout) but would like to get it done in solidworks. I have attached the drawing that i made and would like any help on maybe what i mite be doing wrong.

Thanks in advance,

Brian

[scubanick]

to unfold it it needs to be a sheet metal part
a normal swept pattern is not goin to do it
u can either redraw it trying to make it a sheet metal part first
or convert this boss/base feature to a sheetmetal part
probably easier to start off drawing it as a sheet metal part
i have had some customers come to me with just boss/base featured parts
and i have to try to convert them to sheet metal parts to get them to unfold

[JerryFlyGuy]

You started on the correct track, however you don't need to do the complete profile [ thickness] of the part, you simply draw a single line profile at the top & bottom and then use a lofted sheet metal part to create your loft. You can find the function at --> Insert/Sheet metal /Lofted Bends

Some trick's I've used are:
1) Use the first sketch [ usually the larger profile] to drive the bottom one.
You'll see I've got const. lines from the center of my part to the ends of the profile, I then put the ends of the bottom profile coincident onto the const lines of the first sketch, this way the ends [or opening] will taper uniformly from top to bottom.

2) constrain the ends of the first profile so they are horizontal to each other, this way the split will be centered. I use a dim [not angular] between the end points to control the width.

3) Lofted bends doesn't use K factors so draw your two profiles at your calculated K factor, this only really matters if your doing stuff that is 1/8" or thicker.. If you don't take this into account your part will end up being to large or small depending if you used an inside or outside profile.

4) I've also drawn the profiles [ depending on the situation] as a bunch of equal length straight lines that have all their end points coincident on a const. circle. The circle drives the overall size of the profiles, you have to fillet each line joint, but you will end up with a part that better represents how it will look once broke. Remember to use the same fillet size on the bottom sketch as on the top or things will get wanky on you.

There's lots of other little nick-nak's but this will get you started.

If you want the Lofted Bends on your tool bar, find an area of your tool bars which is blank and right click.. go down to the bottom at"customize", then the "commands" tab, then cycle through the list of commands levels until you find "sheet metal" , find the lofted bends icon and drag it onto the toolbar you want it on.. and voila..

Jerry

[phatfred8]

Hello,

I will try what you have posted after i reply. I am using solid works 2000 and do not have the loft bend. Just add bends. The guy that asked me to look into this has solid works 2006. I have seen the button on his system but do not have much time behind the drivers seat. I will forward this on to him.

Thanks for the help,

Brian Muenchau

[JerryFlyGuy]

I think you can get insert bends to work, but.. and its a big but.. you'll have to take the profiles and add a straight segment into them. This segment will then need a fillet into the curved profile. If you taper the straight segment proportionally from top to bottom and then loft it "thin" [ or w/ a full drawn profile.. either will work] you should be able to click on the straight/flat segment of the cone and "insert bends".. its a work around... i've never had to use it but.. its possible..

It's been a few years since I drove 2000.

Jerry [learning something new everyday..]

[phatfred8]

Jerry,

I been meaning to post a picture of a finished part for you to see. My friend and me made 8 total. Material was 6061-t6 and after I did the welding he sent the parts to get anodized. Turned out real nice after the learning curve was traveled. Draw the part, Cut out the part, make dies for the press brake, procedure to bend parts right, the fit and weld. Bending the cone was 15 bends per half and depth setting ranging from .030" to .078" per hit. I rolled the cylinder on a 36" Wysong slip roll, that was the easy part(7" dia. x 22" tall x .062"). But when it was all said and done it was pretty cool.

Thanks for the help Jerry,

Brian

[JerryFlyGuy]

Hey no problem.. I get a kick outta helping others, I don't know it all, thats for sure, but if I can help... well.. it makes a fella feel good

Jerry

[mattpatt]

Concerning unfolding cones. The actual design and unfolding is not too big a problem. But I've been thinking about the k factor.

Let's say my cone uses 1mm steel. The large diameter is 100mm (OD), small diameter 30mm (OD), centreline length is 200mm.

I've not really played with the k factor, but it seems to make a lot of difference.

I've been using 0.5 as the K factor, but surely is won't be a constant number due to the difference in the bend radii. And if I change the factor to 1 then the actual flat pattern output comes closer to the truth

I guess the best way is to roll a bunch of cones and work out some numbers, or there's the lazy way and ask what others are using.

Any help appreciated.

Matt.

[JerryFlyGuy]

The actual 'book' value for K factor while bending w/ a standard press brake is 0.42. Most people use 0.50 because it's easy to calculate [it's what they've always used when doing things by hand calculations etc]

There are other things which come into play when breaking complex shapes. Die placement overlap, top die taper etc. Also some people would set up and roll cones [yours is probably too small to roll] but when rolling sheet metal I've had all kinds of variations from cut parts and it's all due to operator technique. Some operators put so much pressure between the rolls that the part actually rolls thinner [think rolling out dough] while the next person doesn't have this problem. It can cause serious issues when we laser cut parts and then roll them in a production environment.

Keep in mind also that there will be serious effects on placement in the dies while forming. If I'm off by 1mm on a cone which is 300mm at the minor diameter I'm off by 0.3%, if you do the same w/ your cone you'd be off by 3.3% which will make a huge difference in the accuracy of the final product vs the initial cut part and this could be interperated as a k factor issue.

fwiw

J

[mattpatt]

Thanks for the reply. All good info.

For your info, the cones are hand formed by 'teasing' them around a tapered anvil, or through my home made tapered rollers.

Anyway, the actual cone I'm working on is 97 OD large dia. and 31mm OD small dia. Length is 200mm.

I made a card template and cut the (1mm) steel following this pattern, which was generated at K=1. The rolled cone came out at 98.5mm OD large and 32.5mm OD small. Unsurprisingly (following your comments) using a K=0.5 the rolled cone came out pretty much spot on. Definitely close enough for what I want.

For your info I'm designing the cone using a revolved profile, but revolving it 359.8 degree. Tried a couple of other methods, namely boss/base loft and then cut/extrude and thin a single line to make the cut, then sheet metal bends. Also using sheet metal lofted bends on two sketched open profiles. All seem to work in their own way, depending on the cone diameters and angles and the gap cut in the cone to make the unfold possible.

I'm happy now.

Thanks for all your help.

Matt.

[JerryFlyGuy]

Typically for cones I'd use a lofted bend as I find it to be the quickest. One thing to remember when using lofted bends is that the drawn geometry is assumed to be on the 'k factor' line. The graphical representation of the loft is then off a little bit [as it's either offset outside or inside the geometry line], but the calculated values of the flat layout will be alot more accurate. At least thats how it was a year or two ago.. I haven't stopped to test it since the last couple releases.

J

[mattpatt]

Thanks J. I'll give that a go and see how we get on.

FYI I'm using SW2007.

Matt.