Forming Tools for Sheet Metal

daveaseeman

Hi all,

Has anyone figured out a way to create sheet metal features with complex/curved surfaces other than basic bends and flanges? Thinks like louvers or other formed features?

The approach to modeling is very different than in Solidworks, which is what I'm used to. But I tried here to do it in what I thought might be the Onshape way, but with no luck. The first tab shows the approach with flanges in the center of a part, while the second tab shows how I tried to create a formed feature in a similar manner.

Thanks in advance!

Dave

emagdalenaC2i

Here you can see the formed feature that you try to create.

1. Create a sheet metal model
2. Finish the sheet metal model. So, the forming tools will not shown in the flat model
3. Create the forming tool base part
4. Subtract the forming tool base part to the sheet metal part. You can use "Keep tools" in the boolean feature.
5. Shell the forming tool base part. Set the "Shell thickness" equal to the sheet metal thickness, and remove any face that you want
6. Join the two parts with a Boolean feature
7. Create the fillets. You should create one fillet with radius R and the other with radius R-thickness or R+thickness
   

bryan_lagrange

This is what I came up with:

https://cad.onshape.com/documents/9da6a5d6e4ce2ce60d83ddd5/w/970ad634ad96dad4d69c0622/e/df2eec05c0659f0b4f9e6801

Since I only need a line for a .dxf I made a cut very small in width (.0005"). This contour is small enough that when the .dxf was called into Sigma Nest it saw one single line. 

I completed the sheet metal part then added the louver feature. Since I only need the depiction of the louver in the model and only the cut line in the flat this method worked out best for me.

Hope this helps.

NeilCooke

Look in the FeatureScript examples (+ menu top right to add features to your toolbar) - I added an embossed foot feature. This does require the sheet metal model to be "finished" first. 

BLeeVN

Has anyone taken the time to expand on @NeilCooke Embossing FS to use Multiple Points to generate a Polygon instead of the Sketch Circle?

mahir

Several examples are laying around. Here's a feturescript I made for round embosses/feet. It will work with sheet metal, but only after finishing the part. So emboss features won't show up in the flat pattern.
https://cad.onshape.com/documents/c906e2264d158509753b1bdb/w/54ac31d75d8897024a9c9c68/e/f07b5f8cd8f7543b972b1779

lana

Please notice that sketches in flat can be used to mark placement of formed features. These sketches can be included in direct DXF/DWG export of flat pattern or inserted into drawings.

michael_bass

Thanks for sharing that @mahir !

MBartlett21

@daveaseeman
@michael_bass
@lana
@mahir
@BLeeVN
@emagdalenaC2C

I have just made a forming tool FS: https://cad.onshape.com/documents/a752e0db24eb071ebb6f5aa0
Please try it out and let me know what you think

lana

@mbartlett21 Looks great! That implementation is very close to what we have in mind, except that we'll have to do some work so that calling sheetMetalEnd will not be necessary and there will be some representation of the formed tool in flat. So if users of this feature build a library of configured forming tools, they will be able to keep using it when native forming feature becomes available.  

owen_sparks

How cool is that?

O.S.

Jake_Rosenfeld

@mbartlett21

Excellent use for reference parameter! Nice feature!

xphilip

@mbartlett21 - We are impressed

xphilip

@mbartlett21 - I meant to do that as my 'Onshape' ego.
"We are impressed!"

lana

@mbartlett21
I took a liberty of adding processSubfeatureStatus() call after sheetMetalEnd. This causes a blue info message about changes not being reflected in the flat to appear when the Form SM feature is edited.
 If you agree with this change please release another version. This might save us some support questions from this feature users in the future. Thank you for helping us with sheet metal functionality development.

MBartlett21

@lana

Thanks!

I have released the version as V 0.1.8

MBartlett21

lana said:

@mbartlett21
I took a liberty of adding processSubfeatureStatus() call after sheetMetalEnd. This causes a blue info message about changes not being reflected in the flat to appear when the Form SM feature is edited.
 If you agree with this change please release another version. This might save us some support questions from this feature users in the future. Thank you for helping us with sheet metal functionality development.

@lana
This does not seem to display a popup anymore.
I also tried using reportFeatureInfo(context, id, ErrorStringEnum.SHEET_METAL_END_DONE);, but it did not work either

lana

That is curious - looking. Narrowed it down to presence of populated Part Studio reference parameter. Will pull a bug. Thank you for paying attention

MBartlett21

@lana
Thanks!

nick_papageorge073

Hi, I found this old post from 2019. Has OS integrated any sheetmetal forming tools now? Thanks.

René_Sartorio

Hey @MBartlett21 ,

my goal is to rebuild the embossing library tools from SolidWorks in Onshape.

I found your feature script and am trying to apply it.

https://cad.onshape.com/documents/a752e0db24eb071ebb6f5aa0/w/47c6a6888718e30c80f1f652/e/942b8c71966a4d99ad3d20ce

A few questions I have:

1.       What is "Transform 1" for?

2.       I noticed something else with my test document. There is material that does not belong there. How can i fix it? 

https://cad.onshape.com/documents/c9eb78ae37ac1a81184f65a2/w/8aa655ad7cea7dc1ec6a7ff6/e/361d328b19705a7521903440

3. How to make it known in the flat pattern?


4.Can you control the rotation ? As in Solid works as an example.



5. And the last question. Is it possible to configure a tool in different sizes?




greetings

MBartlett21

@René_Sartorio

René_Sartorio said:

[...]

1. What is "Transform 1" for?

Transform 1 wasn't for anything special. It was just an edit to test if Onshape's thicken worked for it.

2. I noticed something else with my test document. There is material that does not belong there. How can i fix it?
https://cad.onshape.com/documents/c9eb78ae37ac1a81184f65a2/w/8aa655ad7cea7dc1ec6a7ff6/e/361d328b19705a7521903440

That is now fixed in version 0.3.2. The FeatureScript was trying to thicken the material in the wrong direction first.

3. How to make it known in the flat pattern?

Unfortunately, there is no easy way for me to transform a point from the model to the flat pattern so I can place something there. (This may be forthcoming from Onshape)

4. And the last question. Is it possible to configure a tool in different sizes?

Tools can be configured with the Part Studio configurations, just like anything else.

René_Sartorio

I am surprised how quickly the answer came. It (Nr.2) works 
But you have to make sure that all cutouts are made in the sheet before you use the embossing tool. 

René_Sartorio

In my example the configurations work now. Yeah! 

But what if the tool has to be turned around? How can I do that ?

mahir

René_Sartorio said:

But what if the tool has to be turned around? How can I do that ?

It looks like @MBartlett21 's FS has "flip" and "change orientation" options, both of which are configurable. If you need to dial in a specific angle, you can use a rotated mate connector. But if you want the angle to be configured, you will have to create the MC separately since it seems that any MC's created internal to a feature are not configurable.

Eugen

  

Hello @MBartlett21 

I´d like to know how to position the formtool "Kabelbinderbrücke" to my part.
It works by using the sketch point but the mate connector is not accepted.

thanks for feed back
Andreas 

Axel_Kollmenter

Hello @MBartlett21

I need your help. I used your Form Sheetmetal FS but I want to flip the embossing to the other side.

The checkbox "flip orientation" doesnt work. What should I do?

Here is my document: https://cad.onshape.com/documents/16c87fe5481959bfd82b2240/w/589df9a38b2a351384cb1eb2/e/51db203bbdfb1fa367cf9751

MBartlett21

Hello Axel,

I have just made a version 0.4.1 that adds a Flip Z checkbox and renames the Flip Orientation checkbox to Rotate 180. I have also got the feature to now work in feature patterns.

Axel_Kollmenter

Hi @MBartlett21 we need your help again.

We are in the process of implementing our release process. We noticed that the properties in a sheet unfolding are lost due to your feature script. Here we always get an error in the release candidate. Can you optimize your FS so that after using your FS the sheet metal part is still recognized as a sheet metal part. (So the features drag along and the release candidate doesn't throw an error anymore).

After the feature script is applied, Onshape no longer recognizes the sheet metal part as a sheet metal part, but as a "normal" part. Is there any possibility to optimize the FS in that direction?

FYI: @René_Sartorio @M_Brehm

MBartlett21

@Axel_Kollmenter

The reason for it being a normal part after is that this FeatureScript does a "Finish sheet metal model" internally, so that it can make non-developable surfaces.

If you don't use the forming feature at all, and just do a Finish sheet metal model on your part, does just that cause problems in the release candidate?

Aside: An explanation of how sheet metal currently works in Onshape:

A sheet metal model is based on a developable surface body in Onshape, with special attributes applied on each edge or corner of it.[1]
When using features that modify the sheet metal, they modify that internal surface body, and then call `updateSheetMetalGeometry`[2] once they are finished. (This is slightly different for adding and subtracting material on the flat pattern, which is handled by an internal feature called `opSMFlatOperation` (not documented))

Because of this, we can't just edit the folded model, since that is only meant to be modified by the `updateSheetMetalGeometry` function.
(And due to the requirement of it being developable, we can't use any of the forms, since by definition they are not developable.)

[1]: sheetMetalAttribute.fs (doc)
[2]: updateSheetMetalGeometry (doc)

Another Aside

With sheet metal, I had to implement my own function to get the attribute after the sheet metal model was finished, since there didn't seem to be any builtin way to do so

// (MIT License)
// Get the sheet metal attribute of the part
function getSheetMetalAttribute(context is Context, partQuery is Query)
{
    const attributes = context->getSmObjectTypeAttributes(
        context->getSMDefinitionEntitiesOutsideSheetMetalFeature(partQuery, undefined)->qUnion()->qEntityFilter(EntityType.BODY),
        SMObjectType.MODEL
        );

    if (size(attributes) != 1)
        return undefined;

    return attributes[0];
}

// This is copied from sheetMetalAttribute.fs and edited to always include inactive models.
// If entityType is undefined, disregard it.
function getSMDefinitionEntitiesOutsideSheetMetalFeature(context is Context, selection is Query, entityType) returns array
{
    const entityAssociations = try silent(getSMAssociationAttributes(context, qBodyType(selection, BodyType.SOLID)));
    if (entityAssociations == undefined)
        return [];

    const allSheets = qAttributeQuery(asSMAttribute({ "objectType" : SMObjectType.MODEL }));
    const allSMDefinitionEntitiesOfType = (entityType != undefined) ? qOwnedByBody(allSheets, entityType) : qOwnedByBody(allSheets);

    var out = [];
    for (var attribute in entityAssociations)
        out = append(out, evaluateQuery(context, qIntersection([qAttributeQuery(attribute), allSMDefinitionEntitiesOfType])));

    return concatenateArrays(out);
}

Axel_Kollmenter

@MBartlett21 thanks for the fast reply. No, if I just finish the sheet metal part with the normal feature, the error wont show