Sheet Metal Design Rules 1

[neilc78]

Hello,

My boss has asked me to put together an overview document on the do's and don't do's for designing sheet metal machines in Solidworks. I know that this is a huge task and everyones situation is different but I am posting here just to collect some points that I can use. I'd also love to hear from people who previously put a similar document together in the past.
Our biggest concern in design at the moment is that when new people come on board designing in Solidworks, that the design their machines in a manner that allows easy changing of variables in the future if something similar comes up.

Thanks,
Niall

 

[tmalinski]

I'm certainly no expert having posted and asked many questions on this forum myself, but I have the same responsibility for our engineering dept. I have been developing over the last several months methodologies that cover most of the kinds off work we do with sheetmetal and standard features and assemblies. We are a contract manufacturer of metal stampings, (progressive dies, jigs, fixtures, secondary machines and automated machines). You are right, everybody's usage with solid works is different. All I can say from my own eperience is gather information from others as you can, but you will need to apply their suggestions to your own test projects to prove them out as you write your process documents. I have found that what seems to be a good methodology for one kind of project may not work well for another. So far I have several methodologies specific to certain types of jobs. Most of the differences are in the approach up front, Top Down or Bottom up? Use skeleton Sketches / planes or not? I am slowly modifying each of my methodologies as I encounter hiccups or better ways to do things as I work on real jobs. I have found creation of documentation for design methodologies to be an ongoing task. Yours is not a question of how to do something with solid works, but rather how to best apply what solid works can do to meet your needs for a particular kind of project.

tom..

Tom Malinski
Sr Design Engineer
OKay Industries
New Britain CT

 

[Nella95]

One #1 rule, that I, myself have run into, is that sheet metal parts should be designed using the sheet metal command with SolidWorks. (Now it is quite possible, to 'extrude' a part, 'break' the corners, 'unfold' the part, then assign it a 'sheet metal base-flange' feature. But - it is sooo much simpler to 'flatten' the part to get a flat pattern when the sheet metal feature is used.

And when using the 'sheet metal' feature, simply draw a single line, the sheet metal properties adds the thickness and depth accordingly to how the user inputs the data.

 

[Heckler]

Naill,

Here is a link to a general guide I downloaded from a website I can't remember. But it's a useful document.

http://multiterra.mooload.com/file.php?file=files/1137108264/Sheet+Metal+Tutorial.doc

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
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_`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford

 

[TheTick]

sheet metal parts should be designed using the sheet metal command

Good practice in many cases, but hardly a good "#1 rule". Some cases it is better to make geometry and then convert. I certainly wouldn't make a rule to force a person to do this. Many top-down design scenarios work better if parts are converted to shet metal after a certain point. I found this especially true in cases where Someone outside the organization is causing unforseeable design changes.

 

[MElam]

And when using the 'sheet metal' feature, simply draw a single line, the sheet metal properties adds the thickness and depth accordingly to how the user inputs the data.

This is one of our rules, other than we state to use single profile instead of a single line. The important thing for following design intent is in how you dimension the profile. Always use your critical dims. Is it inside or outside? (we have 2-piece guards, one pieces slips inside the other). Then make sure the sheetmetal thickness is going the right way. That way if the material changes the critical dims are maintained.

 

[J-C]

Well I just saw that this book was released. I don't know how good it is, but it might be worth looking into.

http://www.sheetmetalguy.com/

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP3.0 on WinXP SP2

 

[Nella95]

http://www.tenlinks.com/news/PR/Sheet_metal/011306_book.htm

Did someone already post that link?

 

[J-C]

Yeah, it's the same. I just posted the direct link to the website for the book.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP3.0 on WinXP SP2

 

[CorBlimeyLimey]

If the sample PDF is showing the preferred method of creating the piece shown, I have to question the authors judgement. The use of the Jog to create the rear leg, although quite valid for SW software, would not be recognised by a sheet metal person.

However, the book looks like it could be a useful reference/tutorial for someone just starting to use SW SM ... providing they have actual sheet metal knowledge.

Just my 2 cents.




Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[SWXVARGURU]

Check out this site.

http://www.sheetmetaldesign.com/

 

[yanceman]

I use a similar format to Nella95, drawing lines and then selecting BASE FLANGE/TAB. We dimension to the inside edges of a "U" shaped sheetmetal panel with side flanges, with the material to the outside of the sketch. We dimension to the inside edge because material thickness tolerances do not affect the formed sheetmetal part's critical dimensions.

Also, I have had problems using models that others have created that started out as a solid box, and was shelled and ripped, etc... I get a warning message under PROCESSED BENDS that tells me it is ok to delete a bend because it is no longer needed. Well, if that bend is active in another configuration of that part, Solidworks doesn't recognize it.

Forming tools are very handy in sheetmetal parts, as well as design tables (if you use configurations).

Equations are great. Make that inside bend radius equal to material thickness devided by 2. Very handy if all you want to change is the material thickness.

With hole patterns, if the spacing is equal, use LINEAR PATTERN, if not use SKETCH-DRIVEN PATTERN.

The list (and possibilities) is endless. Good luck and have fun.

Go Cav's,
Yanceman

 

[engAlright]

We do a lot of very complex sheet metal shapes and have found that the Solidworks sheet metal features work well for relatively simple shapes, but for more complex shapes with strange profiles and compound corners modelling a solid shape first then using Rip and "Insert Bends" works best.

Biggest problem always seems to be the bend reliefs when working with the Top-Down approach. You seem to always have to make a huge hole in the corners in the flat pattern, then fiddle around with an extrude that is exactly the right shape to fill in most of the huge hole. The space that remains must still provide enough room in the bend region for flare when the part is folded up again. There is definetely an art to it.