Best Practices: Sheet Metal Modeling 2

[MadMango]

I think anyone that has been using SW to do sheet metal design has come to several "best practices" conclusions. I am wanting to start this topic in the hopes that others will share thier practices within our community.

1) Insert your Sheet Metal-Bends feature last, after all of your design work is completed.
2) Use Thin-Extrudes when ever possible when you are modeling long channel-like parts.
3) Features like Counterbores and Countersinks should be placed after the Sheet Metal-Bends, unless you know that these features can be fabricated in the flat pattern of your part (punched or stamped in the flat pattern).
4) When parts are designed for fabrication on a laser cutting machine, include small radii at every interesection of 2 lines (inside and outside corners) so the laser doesn't have to pause to change direction.
"Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[dsi]

One thing regarding item number 1. I typically insert the bends first, making sure that the design functions properly. Then, I supress the sheet metal features before doing anything else. When all of the features have been added, the bends get unsupressed. This method should only be used if the bends are independant of the features to be added. For example, if a bend line is dependant on the location of a slotted hole, I would proceed with your development path. DimensionalSolutions@Core.com
While I welcome e-mail messages, please post all thread activity in these forums for the benefit of all members.

 

[BBJT]

MadMango and dsi,
Are you using 2001Plus? If so are you not utilizing the new sheetmetal functionality that allows you to extrude a sketch as a sheetmetal part right from the get go. The reason I ask is I used to be pretty heavy into sheetmetal design up thru SW2000. I now am strickly support and no design. I have not used the new functionality in 2001plus in the real world of design but I have mess around with it and it seems allot easier to manage things like where to put holes and other features.
BBJT CSWP

 

[MadMango]

BBJT, are you refering to my item 2 above, Thin-Extrudes? If not, then I am not aware of this new functionality you are talking about.

DSI, if you insert the Sheet Metal-Bends first in the Feature Manager, how do you make "sure that the design functions properly"? Or are you saying that you get your basic shape modeled first, insert Bends, then suppress it to add all the fine detail? "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[BBJT]

Start a new part. Create a thin sketch in the shape of a Z or whatever. Instead of extruding it pick the base-flange/Tab on the sheetmetal toolbar. It extrudes the thin sketch as a sheetmetal part right from the start. It works pretty slick. Now start a sketch on one of the faces and extrude cut a hole. No more rolling back to add a hole in the flat state, SW now does it for you.

I think the new icons for sheetmetal show up by default on the sheetmetal toolbar. If not go to cutomize and add them in. BBJT CSWP

 

[MadMango]

Wow, nice tip BBJT. I think you have just changed the way I will create some sheet metal parts in the future. "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[dsi]

MadMango:
Yes, I (used to) get the basic shape modeled first, insert Bends, then suppress it to add all the fine detail?

I, too, have not used the sheet metal features in quite some time and did not look into the new functionality of 2001Plus. BBJT, thanks for pointing that out. Like MadMango, I think I just changed my methodology. DimensionalSolutions@Core.com
While I welcome e-mail messages, please post all thread activity in these forums for the benefit of all members.

 

[DetroitPickles]

I have been using the "new" sheet metal features of 2001plus, like BBJT, since I got the upgrade. BUT, it still doesn't do everything like I think it should (novel idea, huh?).

Therefore, some of the stuff I have done is still done easier (or, easier for me) using the old ways.

Point is, the new features are very slick and works pretty darn well, just don't forget the old ways.....(or until SW deletes them)


Mr. Pickles

 

[MadMango]

Building upon DetriotPickles' comment, what is the general feeling for how some of the new sheet metal features affect model size and stability? I think it is understood for machined parts, that the models "perform better" when things such as radii are built into the sketch features rather than being Fillet features.

Is it better (performance wise, not speed) to build your part features using boss-extrudes and cuts, or is it better to use Miter Flanges, Edge Flanges, Hems and Jogs? "Happy the Hare at morning for she is ignorant to the Hunter's waking thoughts."

 

[earlpatrick]

i haven't had any problems with model stability using the sheet metal features. with regards to model size, i haven't done a comparison between boss extrude and base/flange built models. it would be interesting to know. . .

in terms of performance, i find the sheet metal features much easier to utilize for model revision. and (if you trust the bend tables that SW uses) you can have the flat pattern as a configuration to send to your fabricator.

by the by, the sheet metal features are great for any constant thickness model you need to create as that's the only requirement for SW as far as sheet metal goes. for instance, i use it for glass, insulation, aluminum and steel parts.

cheers,

earl

epillsbury@bensonglobal.com

http://www.bensonglobal.com

earl patrick
epillsbury@bensonglobal.com

http://www.bensonglobal.com

 

[Stoker]

In response to MadMango's May 31 post:

Much of the "new" sheet metal functionality isn't actually new at all. You could always make features such as jogs and hems. The difference is that they have made it more convenient by automating some of the things which previously had to be done manually or in more than a single step. It is kind of like the new dome tool, which is essentially a macro to create a loft. Overall, regardless of how efficient the model is, I think that the new tools are good because they make it very convenient to create and edit these features. There are probably very few people who make so many sheet metal features that there will be a noticable difference in performance between a part with the new tools and the old.

 

[MadMango]

I agree that that the "new" features for sheet metal are nice and convenient, and definately beat some of the older methods of achieving the same outcome.

I work for a company where the majority of our product is designed and produced with nothing but sheet metal parts. Out of roughly 500-800 parts for a new project, 90% of them will be sheet metal alone.

One of these days I might actually do a study to see how sheet metal features affect model size and performance, just for my own comfort. I'm sure SW takes system performance and model integrity into consideration. "The attempt and not the deed confounds us."

 

[Scoobystu]

One particular feature I like is the ability to Edit the flange profile. This basically takes you into the sketcher and you can create any shape you like with the flange without having to axtrude or cut anything.

 

[rocheey]

>>the ability to Edit the flange profile.

I 'discovered' this earlier, and Ive used this to make
'parent' parts that are extremely flexible, and can also
get just as tight a joint between faces as if you'd used
the extrude/shell method.

 

[Niallc]

The most important thing to do when modelling sheet metal parts is to have your bend radius, allowance or deduction values correct. By the way for any of you thinking of using a bend deduction table with metric values I think you will find that there is none included with the package. Even though when you go to insert one and you select "mm" the values in the table will appear in inch. Bit of a pain.

 

[YJeepster]

I agree with Niallc that those things are important, but the most important value is that of the sheet thickness. If you are designing a part for a job shop, and want them to be able to use your model, the thickness must be right to there specs. If not they might as well though out your model and start from scratch! The reason is OD's and ID's will change when the thickness changes, possibly causing fit-up problems. As for the bend radius, and bend deduction this can change without changing the flange sizes.

Q: Niallc, when you say bend deduction, are you talking about OBD (outside bend deduction) or K-Factor? ODB should have both english and metric values, whereas K-Factor is a number between 0 and 1 therefore no differance between the units.

 

[Niallc]

Yjeepster - You are right about the material thickness. If you are using equations or design sheets that allow material to change it is absolutley critical that your model is built in a way that allows the material thickness to be increased in the correct direction. Bend Deduction is the difference between the flat unbent pieces length and the sum of the outside to outside dimension of the bent piece. For Example I could have a piece of 4mm material, 92mm long. If I bend this to 90 degrees and measure the outside to outside dimensions they could be both 50mm. Therefore 100mm minus 92 is 8mm bend Deduction. Now if you go to Insert, Bend Tables, New a pop up will appear asking you for units and type. Select 'mm' and Bend Deduction. A spreadsheet will appear but all the values will be in imperial. I checked this out with our Vendor who told me it is an oversite. Guess i will have to change it myself to metric.

 

[DetroitPickles]

You can fix that. The bend table that you are getting when you hit "New", is the "default" bend table.

In directory "\ProgramFiles\SolidWorks\Lang\English\Sheetmetal Bend Tables" there is 2 files there. One is the "Base bend table", the other is the metric one. Change the metric ones name to the other ("base bend table&quot and you get that one when you click "New". Modify your metric "template" if you want...

Hope it helps...

Mr. Pickles

 

[YJeepster]

Niallc - So you are talking about OBD. Sorry, but I have never used a bend table in SW. I always set-up my bend info in the Insert Bend dialogue box. I haven't used much of the sheet metal features in SW. I found it was faster for me to make the part and then add the bends (Insert Bends) last. This also gave me way more control over my relief notching.

I have been working for a sheetmetal manufacturing plant for 8 years now, and somethings SW wont let you do in sheet metal, you can do in the realy world.

So, I guess my answer to the original question is add sheet metal last. One part I got awhile back total floored me. One customer had actually put fillets on all the bends insted of adding the sheetmetal. Then when I went to remove the fillets all the holes were children to the fillets. What a mess!!

 

[Niallc]

Thanks Mr Pickles, I'll try that. Yjeepster - I know what you mean. We have been bending parts here for 25 years and I am discovering now that some of these bends are theoretically impossible. However I do always try to use the new sheet metal features as I go along because changing all to sheet metal at the end puts doubts in my mind about how parts will line up and so I feel I have to go back and check all the bends and allowances etc.