Hi Community,
right off the top of your head: What is missing in SolidWorks sheet metal functionality and why is it missing (but you definitely can give it also a thorough thought )?
Please share your thoughts and ideas about missing (or areas that need to be improved) functionality. I am curious to get your input...
Kind regards
Frank
Product Definition Team
Thanks for the opportunity! I would suggest you allow me to enter one bend allowance for joggle bends, it is not two bend deductions. The amount the part shrinks is the bend allowance. This of course is desired for joggles where both bends are formed at the same time with one 'hit'. I find it difficult to edit the allowance to some unknown number to get it to be right 'in the flat'. Some may use the joggle bends feature to create two bends in close proximity. When it is two bends we can use two bend dedcutions or allowances.
Hi Bernie,
thank you for your proposal. So you are saying, a jog feature with two very close bends should be treated as one bend?
Thanks
Frank
Product Definition Team
Frank,
Yes. I make this comment based on 40 years experience in the precision sheet metal field actually doing the work in the engineering, fabricating and programming capacities. In the case where the two bends are being formed by one tool in one hit we typically test bend the shrinkage in the specified material. We might start with a piece that is two inches wide and 6 inches long. We accurately measure the blank length, then make one hit to achieve the form.
We then remeasure the length. The difference is the allowance that is added to the blank to compensate for the shrinkage of the form. SolidWorks currently has the "fix length" button for joggles. I believe the simple solution is to allow us to specify what that allowance is that actually causes the 'fix length' condition.
For joggles that are not actually formed in one hit or two bends in relatively close proximity two bend allowances or deductions might be used. I currently use the educated guess that if the inside to inside dimensions of the joggle is less than three times the material thickness I would use one allowance rather than two bend deductions.
I have attached a text file that has been in use for the better part of those 40 years and is very accurate. You may use this for reference as it may help your team. Feel free to contact me again if I can help or you have any questions.
Regards,
Bernie
Update:
Sorry guys/gals, I missed an important fact the the statement here "inside to inside dimensions of the joggle is less than three times the material thickness" I did mean that inside tangent to the bend radius to the inside tangent to the bend radius. We all know that could really have an effect on things.
Message was edited by: Bernie Daraz
Good afternoon Frank,
Great for you to bring this up,
The biggest issue is in the Lofted Bend feature, anytime I design a lofted sheet metal transition that isn't parallel top and bottom, the model is distorted and the flat patterns aren't true. If there is a special transition that we need to manufacture, I can develop it for the model and assembly, however I need to go to another program to create a true flat pattern. Most transitions are created from a top plane sketch and another sketch on a plane that is parallel from the top plane, this works fine, but if I need to have the second plane on an angle from the top plane then the part is distorted. Furthermore each edge that is off the top plane is a spline rather than a straight line as it should be, so I have to go back and add a extra extrude to make that edge straight, see the attached part.
I know we had a few emails going back and forth on that and I think there is a ER on that.
Also, another thing we had discussed was taking a flat dxf file and being able to extrude it flat and add a bend to make it a full circle part.
Bernie, great idea, that would be sweet,
Later,
John
John,
I've been lucky and have not needed the lofting but the joggles drive me mad as soon as I know I need one! I agree with you on the rolled flats too.
Not an insult but it's (sheetmetal) not the same as machining. Aside from cutter issues you usually get what you design and forward to the machinist. With sheet metal there's so many tiny and major variables. It's no wonder no one has an add in that runs inside of SW to program turrets or lasers al a MasterCAM and the others.
One more would be that we should be able to add flanges on the edge of rolled cylinders. I understand that SW wouldn't flatten them correctly. Maybe they could do something where we could add a flatten feature, add the flanges and then tell SW to ignore the issues in the compound bend region. At least that way we could forward our flats to the directly to the lasers or turrets.
Bernie
Hi Bernie,
thank you a lot for your insights and detailed explanation. I really appreciate your feedback! Recently I was talking to a customer in Germany and he explained almost the same requirement to me. So it seems to be something international...
Thanks
Frank
Product Definition Team
Hi John,
yes, the lofted bend issue is a known issue and we are aware of it. When I look at your part, I am actually wondering how it is manufactured. Is it really manufactured as a "formed component" (kind of a die formed part) or is the shape approximated by several differently angled bends?
Thanks
Frank
Product Definition Team
Hi Bernie,
yes, adding flanges to circular edges is also a known issue.
Thanks
Frank
Product Definition Team
Here are a few to chew on.
1. Allow the use of a plane reference for Unfold/Fold sequence. The way it is, if you Unfold and then cut off the edge that was the ref, you have to fold along a different edge - if you even have a straight edge left. Either way the part moves.
2. Allow the ability to remove the first selection in a multi-select edge flange. Currently you can't remove that one.
3. Allow edge flanges to be pulled out past their base.
4. Try to improve close corners on miter flanges. It currently will only close straight portions.
5. Improve the rebuild time on closed corner of cousins. Closed corner of brothers (same parent) works pretty well, but the new closed corner that will go all the way out is handy but takes a rebuild hit.
WT
Here is another to chew on.
We have a 3d surface like a wavy washer. It is a formed shape. It could be sheetmetal. It is formed though.
So we need to flatten it out.
If you did it would tear or stretch in some areas and shrink in others. So there are no bend lines to unfold.
It could be a sheet metal part but the SW sheetmetal tools are not what you would use to flatten it.
We did try to do a projection of the shape and then scale changing the X and Y aspect ratio.
Anyway someone here smarter than me might be able to state what SW enhancement makes sense.
Good morning Frank,
Our guys on the shop floor will add a certain amount of bends from the long edge side corners and do a slight angular bend across the part.
Later,
John
Hi John,
thanks for the clarification.
Thanks
Frank
Product Definition Team
Hi Wanyne,
1. I suppose you are talking about cylindrical, conical parts where you use the insert bends command. You have to specify a fixed edge and when you cut that edge away you are in trouble...
2. As far as I can remember this was fixed with 2011. I just double checked in 2012 and it works there.
3. Yes, I can see the benefit of this enhancement...
4. Can you give me an example for this? Unfortunately I am struggling to imagine the type of geometry...
5. Sorry, but I am also struggling to imagine the geometry. So can you please give me an example?
Thank you very much in advance for your additional business.
Thanks
Frank
Product Definition Team
Hi Jerry,
thank you very much for your response. I can see that it might be handy to develop formed sheet metal components. But as you pointed out there will be some areas where the material gets compressed, respectively stretched.
Would you expect to get a display or a report of the stretched/compressed areas? Bottom line I am asking if you imagine a sophisticated algorithm that takes the material parameters into account and can calculate the material stress or if it would be sufficient for your needs to just "unfold" the curvy surface?
Thanks
Frank
Product Definition Team
I just needed to unfold it. That would be a good start.
1) need ability to "use a plane" for edge-flange perpendicular & parallel reference.
2) need ability to "use an edge" for edge-flange parallel reference.
on a side note, most people would choose a lofted-bend for this.
the downside with lofted bends is they do not depict real world results.
if this part was done as a loft, the sides would be twisted or helical.
there is no way to replicate that in the real world.
Hello,
Here are some basic ideas.
Lofted sheetmetal, convert to sheetmetal -> make the "link to thickness" option available.
Sheetmetal bendlines in drawing views - The visibility is tied to the "show/hide sketch' setting. An option to show the bendlines & bend notes indepent of the sketch view settings would be awsome.
Ability to link gauge designation to custom property i.e. select gauge size from table and have gauge description & thicknees available as linked custom property. If this was available for multibody sheetmetal and cutlist properties would top the list.
Being able to flatten sheetmetal by selecting any edge and or a reference plane. Currently the edge has to be straight or you need a flat face. Lofted sheetmetal often has no "real" flat faces i.e. square to round eventhough the triangular shapes are mathematically flat.
Mirror sheetmatal body is only working if the face selected connects to a flat surface. Extend the mirror body command to accept any
sheetmetal face (faces parallel to thickness only of course).
The reference plane would be great cause currently you can unfold/fold a sheetmetal only if the selected base face remains available in case I add a cut feature in the unfolded state. If the cutfeature happens to remove the orig. face - > no folding operation possible.
Autopopulate flat layouts for multibody sheetmetal.
Setting to show single body sheetmetals in indented BOM's as single line item. Currently you get a line for the part and a second line for the body itself. Unless you have a cutlist folder however you can't get the automatical calc. sheetmetal blank sizes.
In case I change the material on the formed part, I want the material also to strictly change for the flatten version. Never seen a part that was cut out of material A and then magically formed into something made out of Material B . I am not sure if this is fixed, but when using the property tab to change material type, this can cause havoc especially if display states are being used. You end up changing the material only in one configuration unless you open the material selection box and "open & close" the apply to all config dialog box.
Autocreate a 1:1 scaled flat pattern on a seperate drawing sheet with specified name (should be customizable) i.e. DXF or flat pattern.
The current export dxf does this already in the background. It would be great to stamp it also with custom properties automatically like size, material etc. and add overall dimension. This will allow you to batch export any dxf in the future (time saving) including updates and design changes and also check the flat pattern before cutting (very important!!).
Edge flange - editing the edge flange won't allow you to delete the first (initial selected) edge. Would be nice if that limitation was removed.
I am still running 2010 and maybe some bugs mentioned are fixed but for most part i think that would result in time savings.
Thanks,
Elmar
Hi Kenneth,
thanks a lot for your feedback.
Yes, I can see the requirement to use a ref plane or an edge in order to specify the angle of an edge flange.
Thanks
Frank
Product Definition Team
Hi Elmar,
thank you for the comprehensive list. Seems to be a list of smaller issues but they would end up as huge time savers.
I am struggling with the "link to thickness" option as it is active in my 2012 (at least for cut extrude/boss extrude).
Thanks
Frank
Product Definition
Hello Frank,
If you have a "thickness" value defined in your template then SW will give you the check box "link to thickness" for cut extrude, boss.
Well let's say I use lofted or convert to sheetmetal features as my bose feature for the sheetmetal part then this option is not available.
I can however in a secondary step double click the lofted or convert-sheetmetal feature, select the thickness and link it to the existing "thickness" variable. If i don't do that than you can manually enter the thickness for the base feature independant from the global variable.
The check box would enforce a uniform thickness and simplify that step.
Thanks,
Elmar
would be nice to do transitions like real life and not the way a loft does them.
Ok, thanks for the explanation. Now I have got it.
Thanks
Frank
Product Definition Team
Hi Kenneth,
how important would it be that all bends meet in one point (the corner of the rectangle)?
Thanks
Frank
Product Definition Team
they don't meet at the same point.
just very closely spaced to give the illusion of one point.
i just upgraded to 2010 sp5 from 2008 and I've noticed the changes in sheetmetal functions. We make alot of big roll-ups with holes cut in them for nozzles. In 2008 I would use normal to cut and flatten the roll-up and be able to plasma burn the size OK. In 2010 the normal to cut-feature has changed. It makes the nozzle hole to large. Maybe this has been resolved in 2012?
Below is the roll-up, 106 OD, 5/8" thk, nozzle holes are 36 OD
the arc length from AutoCad
Solidworks flat pattern with normal cut on about 1" big
normal cut off - not ideal for flat pattern burnouts
sorry for all the pics, just wondering if this still happens in 2012?
on Jun 27, 2012
Thanks for the opportunity! I would suggest you allow me to enter one bend allowance for joggle bends, it is not two bend deductions. The amount the part shrinks is the bend allowance. This of course is desired for joggles where both bends are formed at the same time with one 'hit'. I find it difficult to edit the allowance to some unknown number to get it to be right 'in the flat'. Some may use the joggle bends feature to create two bends in close proximity. When it is two bends we can use two bend dedcutions or allowances.