CAD Forum

I would like to know your best practices for sheet metal parts regarding some points.

1. How do you create them? Do you omit sheet metal features on purpose?
2. How do you mirror them?
3. How to organize them in an assembly regarding
   1. multi-body sheet metal parts (do you use them?)
   2. mating them without breaking those mates after editing
   3. mirrored parts (patterned or not?)
4. How do you set up the hole wizard feature within sheet metal parts?
5. How do you handle parts that have many (bump) bends in them or that are flexed to fit for the BOM?
6. How do you handle those parts for different sheet sizes & what about the seam position there & the BOM?

What we currently do:

1. Our supervisor insisted to put everything into a drawing at first, but we are now allowed to use more features. Most of our parts have only two features though: Base-Flange & Sketched bend.
2. I personally use mirror->keep body to set them up, but everybody else repeats all sketched bends to the opposite direction to make it work:
3. 1. We do not use them, because we could not get it to work properly on our BOMs
   2. Supervisor does not care, so most of the time I have a very red assembly. I tried fixing that through the use of envelopes with mediocre success, because again - 90% of the time nobody except myself mates to the envelope (they are too lazy)
   3. A total mess up. I found, that mirroring parts with a pattern only works well, if you use mirror->keep body properly. Otherwise you have to insert the part twice & add symmetric mates all the time.
4. Since we were not allowed to use this feature for a long time, we did not use it. Now that I tried it out, I realized, that it does not work nicely on mirrored parts. Any idea on how to solve that?
5. We make them have a lot of sketched bends for bump bends. A total disaster for performance though. And for flexing parts we make a configuration to refer to for the BOM.
6. We put them into the model to double check for problems regarding the seam positions. It just makes the model HUGE, because we have SO many different sheet sizes for various parts. Any advice on that?

I'd appreciate any insights from you. Also just part answers or examples. I'll try and upload some pictures later today.

Edit2: They closed down my department (outsourcing) unexpectedly with a very short notice, so I'm currently not able to access anything sex related (No active license anymore...) I hope I will be back soon, but it will take some time, because I currently do not own a working graphics card (was searching for one, but the prices are insane right now). Sorry for this late answer!

I should mention right here, this being a good place to do this, that there is a way to bookmark posts.


You can then access your bookmarks in the User Control Panel, Overview, Manage Bookmarks

berg_lauritz wrote: ↑Tue Mar 16, 2021 1:12 pm I would like to know your best practices for sheet metal parts regarding some points.

1. How do you create them? Do you omit sheet metal features on purpose?

I design the sheet metal part as it should be in the final product. I then create different configurations depending on need. For instance we don't put in threaded holes even at the minor diameter because we've had problems with material hardness.

All sheet metal parts will have a flat pattern config that will be as it is cut laser/flame/Jet etc.
All Sheet metal parts have a "As designed" config
If need intermediate configs are added for things like "Pre-machined" parts that need features prior to bend that can't be in the original template
If needed same as above for post bend.

berg_lauritz wrote: ↑Tue Mar 16, 2021 1:12 pm
[*]How do you mirror them?

I don't use mirror of anything except sketch entities in solidworks. I've had WAY to many cases of odd mirrors that have caused problems.

berg_lauritz wrote: ↑Tue Mar 16, 2021 1:12 pm [*]How to organize them in an assembly regarding

1. multi-body sheet metal parts (do you use them?)
2. mating them without breaking those mates after editing
3. mirrored parts (patterned or not?)

"Multibodied parts" are almost always going to be weldments in my case. So I create a weldment and put bent sheet metal parts in that weldment. From there I create configurations that are of the above but only have the individual sheet metal parts. That way I can create drawings of individual sheet metal parts that are used in the weldment. That is how the below part was created which is a mixture of bent sheet metal and plates.

Mates break in SW no matter what you do short of not using mates to anything that is not a base plane or something like SSP....and again I refuse to use mirror.

berg_lauritz wrote: ↑Tue Mar 16, 2021 1:12 pm [*]How do you set up the hole wizard feature within sheet metal parts?

Not sure what you mean here? Hole wizard wouldn't change for sheet metal parts unless for some reason you have a specific wizard set up for sheet metal parts. Personally I wouldn't approach it that way rather I would add a "Sheet metal" standard to the existing hole wizard if you had a whole lot of sheet metal specific features.

berg_lauritz wrote: ↑Tue Mar 16, 2021 1:12 pm
[*]How do you handle parts that have many (bump) bends in them or that are flexed to fit for the BOM?

[*]How do you handle those parts for different sheet sizes & what about the seam position there & the BOM?
[/list]

Again not quite following but to me it doesn't matter how complex or simple the part is you should follow the same standard approach.

MJuric wrote: ↑Tue Mar 16, 2021 1:43 pm

berg_lauritz wrote: ↑Tue Mar 16, 2021 1:12 pm
[*]How do you mirror them?

I don't use mirror of anything except sketch entities in solidworks. I've had WAY to many cases of odd mirrors that have caused problems.

If I may jump in, I hear that a lot about mirroring = bad in SW. Can you clarify if you are talking about mirror feature within a file such as mirror body or a feature, or are you talking about one file is a mirror of another file. The latter being select a plane then Insert->Mirror Part.

We have a lot of right/left parts, modeling and then maintaining both would kind of stink.

Now I too have found mirroring features to be sketchy business. On the other hand mirror body was a encouraged method of modeling symmetry, nothing conveys the design intent of symmetry like a mirror body feature. If mirror bodies in SW is a bad practice I'd like to know about it ASAP!

Thanks.

I strongly disagree with the statement about mirroring being a bad thing, especially for mirroring bodies.

This, IMHO, is the order of mirroring stability in SWX from best to worst:

Bodies / Components
Features
Sketch Entities

Mirroring features might fail sometimes on creation (Tab-Slot is notorious) but I've never had it break later. Mirroring bodies is WONDERFUL. Like @bnemec said, nothing spells design intent like a mirror feature towards the end of the tree.

bnemec wrote: ↑Tue Mar 16, 2021 3:27 pm

MJuric wrote: ↑Tue Mar 16, 2021 1:43 pm

berg_lauritz wrote: ↑Tue Mar 16, 2021 1:12 pm
[*]How do you mirror them?

I don't use mirror of anything except sketch entities in solidworks. I've had WAY to many cases of odd mirrors that have caused problems.

If I may jump in, I hear that a lot about mirroring = bad in SW. Can you clarify if you are talking about mirror feature within a file such as mirror body or a feature, or are you talking about one file is a mirror of another file. The latter being select a plane then Insert->Mirror Part.

We have a lot of right/left parts, modeling and then maintaining both would kind of stink.

Now I too have found mirroring features to be sketchy business. On the other hand mirror body was a encouraged method of modeling symmetry, nothing conveys the design intent of symmetry like a mirror body feature. If mirror bodies in SW is a bad practice I'd like to know about it ASAP!

Thanks.

Mirror entire parts is what I have tried most in the past...you know because Inventor did that flawlessly :-)

I think Michael was the one that mentioned mirror bodies instead and I have not tried that.

mike miller wrote: ↑Tue Mar 16, 2021 3:33 pm I strongly disagree with the statement about mirroring being a bad thing, especially for mirroring bodies.

This, IMHO, is the order of mirroring stability in SWX from best to worst:

Bodies / Components
Features
Sketch Entities

Mirroring features might fail sometimes on creation (Tab-Slot is notorious) but I've never had it break later. Mirroring bodies is WONDERFUL. Like @bnemec said, nothing spells design intent like a mirror feature towards the end of the tree.

We talked about this on the other forum. I have always attempted mirroring an entire part, not bodies as that was what I did in IV. In my experience mirroring a full part using features is just too dangerous to even do. I've seen WAY to many parts incorrectly mirror with no sign of error or flag to even recommend it as even a usable feature.

Again, mirroring bodies may be different as I've not tried it very often.

I would like to know your best practices for sheet metal parts regarding some points.

How do you create them? Do you omit sheet metal features on purpose?
99% of time i am using sheet metal features.I like to start with base flange and then add flanges etc..
I will often use base flange to extrude profile (not one flat surface only)

How do you mirror them?
I did not notice to much problems with mirroring SM features or bodies (It is kind of annoying that i cant use plane for mirroring body)

How to organize them in an assembly regarding
multi-body sheet metal parts (do you use them?)
I work often with weldments so 99% of the time multibody is my way.

How do you set up the hole wizard feature within sheet metal parts?
No problem with this?

I answered to questions for which i had something specifically to say.

I don't do a lot of Sheet Metal anymore, but at one time that is all I did, everyday - That was before all the new fangled Sheet Metal Components worked well, back before we had a lot of the new features.

So now if I were to go back and do sheet metal, I think I would do it like I did years ago, avoid the Sheet Metal Features as part of the part development, I'd add them at the bottom of the feature tree and not having to worry about altering flange angles or whatever, model it, rip it, bend it... Just my 2 cents,

It really depends how your model looks.
For me starting with "regular" features and then converting it to SM would be nightmare although i have cases where i use that workflow also

Lapuo wrote: ↑Thu Mar 18, 2021 7:35 am I would like to know your best practices for sheet metal parts regarding some points.

How do you create them? Do you omit sheet metal features on purpose?
99% of time i am using sheet metal features.I like to start with base flange and then add flanges etc..
I will often use base flange to extrude profile (not one flat surface only)

Always start with Base-Flange unless you need to do a mid-plane extrude. Convert-SM gets really messy in multi-body parts, AND you're not taking advantage of things like miter flange and jog, etc.

How do you mirror them?
I did not notice to much problems with mirroring SM features or bodies (It is kind of annoying that i cant use plane for mirroring body)

Yes! Yes, you can use a plane to mirror flanges.

How do you set up the hole wizard feature within sheet metal parts?
No problem with this?

To be honest, there is no point in using HW if the part will be laser cut and you don't need to mate a bunch of fasteners. I just use Cut-Extrude or put holes in the Base-Flange feature.

mike miller wrote: ↑Fri Mar 19, 2021 9:43 am To be honest, there is no point in using HW if the part will be laser cut and you don't need to mate a bunch of fasteners. I just use Cut-Extrude or put holes in the Base-Flange feature.

We actually use Hole Wizard for sheet metal parts quite a bit. Reason being that we have panels with electrical components mounting on them and one Hole wizard feature can cover the 4 holes needed to mount a contactor or transformer. Then you can save it as a library feature and drag in as needed, and when it comes to applying hardware in the assembly you have hole wizard pattern to use.

For one off holes that don't get a fastener, we are more likely to use a cut extrude.

To be honest, there is no point in using HW if the part will be laser cut and you don't need to mate a bunch of fasteners. I just use Cut-Extrude or put holes in the Base-Flange feature.

For holes yes maybe, but we have a lot of parts which have threads , slots etc.. And HW is great for that.

1. How do you create them? Do you omit sheet metal features on purpose?
Base usually starting with a centered rectangle at the origin.
When the design warrants it, I will do an open line sketch for the Base.
99.99% sheet metal features. Less downstream issues and less tree backtracking
One part, one file. Rarely use multibody.
2. How do you mirror them?
Using Mirror
Mirror SM features and for creating a separate opp hand part
3. How to organize them in an assembly regarding
a. multi-body sheet metal parts (do you use them?)
Nope.
b. mating them without breaking those mates after editing
Usually no issues with mating as are mostly PEM'd or holes for aligning to PEMs on the mating part
c. mirrored parts (patterned or not?)
?
4. How do you set up the hole wizard feature within sheet metal parts?
Use HW for PEM holes and for screw clearance holes. if it's for a fastener, it's HW, otherwise it's a cut
Bare part is a SLDPRT, PEM'd is an SLDASM of the same name/part #
PEM'd assy is dwg sheet 1 (or more), bare part is detailed on subsequent sheets in the same SLDDRW.
5. How do you handle parts that have many (bump) bends in them or that are flexed to fit for the BOM?
If lofted doesn't apply, then it's multiple edge flanges driven/linked via the Equations dialog
6. How do you handle those parts for different sheet sizes & what about the seam position there & the BOM?
One sheet size (I'm assuming drawing sheet here).
Stock sheet is only a concern for me if it's a large blank. Nesting is by the fabbers.
"seam position"?

Kevin

As others have said, mirroring is solid, and mirroring bodies often works best.

I use Hole Wizard as much as I can to simplify assemblies. I populate fasteners with Pattern Driven Patterns at every opportunity. I will even mirror bodies first and then add a Hole Wizard after, even though this makes more work doing the Hole Wizard. That way the assembly is more straight forward.

Dwight

Don't be afraid to start outside of typical sheet-metal modelling. Some shapes work much better in "normal" modelling and converted at a later point. Z-bend brackets are a good example. Also anything complex that would be better with a layout sketch.

Thank you for the input. My department was closed down last week due to outsourcing & I cannot answer properly right now. It will take some time, before I can add something to the discussion again.

HerrTick wrote: ↑Mon Mar 22, 2021 9:51 am Don't be afraid to start outside of typical sheet-metal modelling. Some shapes work much better in "normal" modelling and converted at a later point. Z-bend brackets are a good example. Also anything complex that would be better with a layout sketch.

Do tell, why would a Z bracket be better to convert to sheet metal? Just curious since I've modeled so many. I've done side profiles of the "Z" and even a flat plate with two edge flanges, but never a convert.

jcapriotti wrote: ↑Wed Mar 24, 2021 12:42 am

HerrTick wrote: ↑Mon Mar 22, 2021 9:51 am Don't be afraid to start outside of typical sheet-metal modelling. Some shapes work much better in "normal" modelling and converted at a later point. Z-bend brackets are a good example. Also anything complex that would be better with a layout sketch.

Do tell, why would a Z bracket be better to convert to sheet metal? Just curious since I've modeled so many. I've done side profiles of the "Z" and even a flat plate with two edge flanges, but never a convert.

I am also interesed in HerrTick opinion.

Most of the Z-brackets I've done connected two members in a with contact on opposite faces of the bracket, sometimes in cases where faces were not quite parallel. This geometry was far easier to design and control with conventional features. Doubly so if you are working in-context.

A better example would be hinges. Hinge design went much better with conventional features, especially considering the specific constraints presented by my employer's processes. The only compelling reason to use sheet metal was if barrels or bends needed to be unfolded to cut special features like reliefs or stops.

1. Depending on the complexity of the design I will either start with a sheet-metal feature or solid modeling and then convert to sheet metal. The more complex (multiple compounded angles) the more likely I am to start off with solid modelling and then convert to sheet-metal at the appropriate point. I find it a whole lot easier in the design process for complex sheet metal work.

2. I use mirror in all aspects, sketch, features, bodies and final parts (lefts and rights). Never had too many issues with it.

3. My go to for assemblies is SSP method, and rarely use multi-body sheet metal parts (we do not weld much), more mechanical assembly type work. Mirrored and pattern parts is a definite yes.

4. I use hole wizard for all holes type. I believe it works just as well as it does on non sheet metal parts.

5. As for parts that have many bends, I guess it's the same as any other parts (use of patterns...) and ensure manufacturability. I am not too sure what you mean be 'flexed to fit BOM'.