Sheet Metal Help Needed

[JimboJones21]

Hello All,

I'm new to this forum and SolidWorks2004. I'm in the process for trying to build a custom computer case for a mini-itx mobo and learning SolidWorks to design it.

I made my sheet metal case, then flattened it, cut my holes and when I UNflatten it all my holes are gone and everything under the flatten symbol is suppressed. If I UNsuppress then the part flattens out again.

Is there any way for me to fold up my part and keep the cuts I made, or do I have to start over?

Thanks for the help,

Ed

 

[Theophilus]

I'm not completely sure, but I think you simply need to reorder your features.

Get familiar with the roll-back ability and roll your part all the way back to the first feature. Then, roll the part forward one feature at a time and see what changes. You'll see that the sheet-metal bends are inserted and there are at least two sheet-metal features to create the bends and flattened part. Study this and determine whether your holes need to be moved to be included where you need them (flat state, folded state, both, etc.).

Once you determine that, you can move your features where they need to be for what you need to have in your part.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[aamoroso]

The holes need to be above the flatten, right now they are depending on the part to be flat to exist. If it is necessary to put the holes in the flat the use the flatten feature, add your holes and then use the unflatten feature.

(If your real name is Steve, ask Aron or Alan to show you, lol.)

 

[hisrik]

Did you start off with a base flange or started as a solid and converted the part into sheet metal?

Sounds like you started off as a base flange. If you are more comfortable inserting holes in the flat, then do not flatten the part and add features. Use the "unfold" feature. So you need to roll your bar above "flat pattern", unfold the part by picking a face and asking it to collect all bends and unfold. then you will have a flat. add all your holes.

Now fold your part using the "fold" feature. then drag down your bar beyond the "flat pattern".

This should fix your problem. Here we should note that Solidworks considers the features added above the flat pattern only.

If you start out as a solid and insert bends at the end, your hole features should be after "flatten bends" and before "process bends". The software looks at it like you are unfolding, adding features and folding back.

 

[JimboJones21]

I started out by sketching a U shape, then flattened it and made my cuts. So now all my cuts are under the flate pattern. I will try your suggestions but I only started using this software a few days ago and not familiar with the software or terminology yet. Thanks for the advice,
Ed

 

[JimboJones21]

I just tried dragging the cuts above the Flat-Pattern and it tells me that I can't put the child feature infront of the parent feature.

 

[CorBlimeyLimey]

If you post a screen shot of your Feature Manager tree it would be very helpful?


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[JimboJones21]

CorBlimeyLimey do I need to post the screenshot on a web server or is there a way to link it to my reply? I figured my question to be, can I move my features over the flatten symbol in my Feature manager, or do I have to use the unfold command and redraw all my sketches for my hole features? Thanks again. I have to say I've never experienced a forum that responds so quickly to questions!! This is amazing!!
Ed

 

[smcadman]

Not sure how you created it, or how far you are, but sometimes it's easier if you start from scratch. Try this:
Start a new drawing.
Pick the Top Plane, then pick your Line tool and draw and dimension the "C" shape. Next, from the Sheet Metal toolbar, pick Base/Flange Tab button, and enter the height and sheet metal thickness and bend radius.

Now, instead of flattening it to put your cutouts/holes in it, just pick the face you want to put features on and pick a tool from the Sketch toolbar and draw your shape. After drawing your shape/hole, pick Extruded Cut and choose "up to next" or "through all".
This is much easier than rolling back and worrying about order of features. Instead of rolling back, choose the Flatten button from the Sheetmetal toolbar to view the flat pattern.

Flores

 

[JimboJones21]

So there's no way to move the features under the Flatten-Part command on the FeatureManager eh. I'll redraw it which, in itself, is a good exercise
I guess the lesson here is if you're going to flatten (or unfold) an object use unfold, not flatten.

Ed

 

[MadMango]

There are two methods to create a sheet metal part; with Base-Flange as smcadman noted, or Insert-Bends. Both have pros and cons, read-up on them in SW Help. You have not really explained which method you used to create your case.

You should have waited to Flatten your part after all your features and cuts were made. It's much easier to design this way, rather than flattening the part and transposing dimensions to place cuts in the folded shape.

I doubt that you can drag the features up and over the Flatten. I think your best bet is going to be to delete the Cuts, but not the feature Sketches. Then drag the sketch above the Flatten and then Cut-Extrude to get your cuts back.

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[MMike1]

This exact same thing happened to me. (I'm new to SW too). I created two nearly identical sheet metal parts, both using the same method. I was insering bends. then I created my holes.


i did the first one with no problems at all. I then created my dwg showing the flat pattern etc etc. But when I got to the second part, all of a sudden the holes in my flat pattern disappeared. I spoke with a buddy of mine and he suggesting creating a second configuration of the part...called "flat"...or whatever. that seemed to fix my problem without having to rebuild. Not sure why it worked. But it did.

 

[hisrik]

Well...EddieRiby..Try this!

After you unflatten it, the part forms up and all the features beneath flat pattern get suppressed. Now go to the first feature after flat pattern, then to the sketch in the feature and right click and "Edit Sketch Plane". You will most likely not find any face selected in your dialogue box on top left. Select the face where you already inserted your holes and rebuild.

(If it shows errors just redimension it..)

Now try dragging your feature above "flat pattern" and unsupress it. This should work. Repeat this for your features below "flat pattern". A lot easier than creating all over.

Hey let me know though..!! Keep me posted. Good luck!

 

[TheTick]

Are you using "Unfold" and "Fold" to unbend-rebend your part, or are you using "Flatten" to activate the flat pattern?

If you need to cut features and then refold for more designing, I recommend using "Unfold" and "Fold".

 

[engAlright]

More along the lines of theTick's thought -

When you use insert bends the last feature in the tree will be "Process-Bends" when you use sheet-metal features (i.e. base flange) the last feature in the tree will be the "flat Pattern". In both cases, this last feature is what folds/flattens the parts for use in the flat pattern configuration as it appears on the drawing. Any features added after these features will be suppressed in the flat pattern.

For features to appear in both the flat and folded:
-put between "Flatten Bends" and "Process Bends" if using insert bends
-if using base flange, and an "Unfold" feature just before the flat pattern feature, add your cuts or whatever, then add a fold operation after those cuts

 

[CorBlimeyLimey]

EddieRiby ... You need to post the screenshot to a web server. There are many free image hosting sites ... the one I use most is

http://www.imageshack.us

As the others have said, it is best to place your features in the bent-up condition & let SW do the flattening for you. However if you have to cut a feature across a bend, then you should use the Unfold/Fold method.


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[JimboJones21]

Hisrik, thanks for the idea but it doesn't seem to do anything. It does move my holes around randomly it seems, but I still can't move the holes over the flatten symbol on the Feature Manager. If I then try to remove the 'Sketch Plane/Face' it then asks me if I want this to be a dangling reference and that makes for some wacky results.

 

[JimboJones21]

Thanks for the info CorBlimeyLimey! Here is an screenshot

http://img113.exs.cx/gal.php?g=soildworks9ss.jpg

 

[CorBlimeyLimey]

OK, first of all, you will have to delete the Extrude1. The Sheet Metal module can only process constant thickness material.

Next, any features which were drawn on the "fixed" face of the part should be able to be dragged & dropped above the Flat-pattern1 icon.

Any features not sketched on the fixed face will have to have its sketch relocated using the Edit sketch plane tool.

Then the feature should be able to be dragged & dropped.

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[hisrik]

Well, I guess you are stuck with the tapped holes! Obviously there is no option to edit the sketch plane here.

But the other features, I do not know why it is not working at your end. I just tested a sample part and it worked. It lets me move my features aboe flat pattern after I do "Edit Sketch Plane" and pick the required face and redimension it if necessary.



Mechanical Engineer