sheet metal mirror problem

Yam_S

Hey,

1. I'm trying to mirror an extrude remove hole.
I can mirror it within the same sheet metal part with "face mirror", but when i try to mirror it to another sheet metal part, it fails.
why ?

in the attached pic the black arrow is the original extrude, the red is the mirrored one.

2. any news about adding "feature mirror" to sheet metal parts ?
is there an improvement request for it ?

Regards
yam

John_vd_Werff

Mirror of a single feature from one sheet metal part to another part won't work.
Assuming you have a 'front' and a 'back' version of the sheet metal part you should be able to design 1 part (either the front or the back version) with all features and then mirror the entire part. If required you can add individual features to each part after the mirror feature

Yam_S

Hey John, thank you for your comment.

The feature I'm trying to add is done after the major mirroring of the part.
After that mirror which was made earlier in the design, a lot of features are already depended on that mirror move so I can't just drag it to the end of the feature tree.

What I did eventually is a mirroring of the sketch, which can be done for some reason, but it's a workaround.
I just don't get why the mirror doesn't work that way.
You have a feature or a face, you have a plane, the software gets it (red arrow), she just needs a "merge scope". seems that its (once again) not that far from being implemented.

eric_pesty

I might be wrong  but it looks like the two faces are parallel, if they are, you could just extrude in the other direction as well to cut both holes with the same extrude.
Or if you can't move the mirror to the end can you move this hole above the mirror feature instead?

Yam_S

Hey Eric,

your first suggestion is interesting, it can be done with the right merge scope.
the second one is not always doable due to sketches that use future reference/ in context.
thank you.

anyone knows something about improvement request in this subject ?

John_vd_Werff

I think the question has much deeper root causes than the mirror feature itself.

Multi-part part studio

Apparently you are working in a multi-part part studio, which can be a very quick and intuitive way to create entire assemblies because it is easy to create relations between features on several parts. This aproach however has several downsides:

- you may end up with models that are very hard to understand later on because everything is somehow related to everything else.

- cross relations between multiple parts that are created on the fly without a general mastersketch can have unexpected results (like canceling out or changing a previous feature)

- release of individual parts and revisions later are hard to manage 

Personally I am a strong advocate that each single part should be designed in a separate part studio, unless there is a complex interaction between parts (as in a hinge, or a 4 bar linkage mechanism, etc.), or parts are mirror versions of each other.

If a multi-part part studio is required than I would advise to keep the features grouped together per part as much as possible (finish all features for the first part before adding features for the second part etc., this does require some thinking ahead and making a general plan of the entire design)

Intuitive use vs fundamental logic

I have used 6 different large CAD applications on a professional level and several others on side projects. On a modelling, assembly and configuration level Onshape is definetly the most robust and stable CAD application I know. But it is not the most intuitive application to use. A good example are the mate connectors in Onshape, the 6DOF connectors are a perfect mathematical representation of the mechanical connection design intent. But you realy need to learn how to use them properly. Other CAD system have far more intuitive ways to constrain parts, but those constraints often result in overdefined (= computationally unstable) assemblies.

Onshape focuses on the implementation of fundamental stable logic for its features at the cost of intuitive use. Modeling stabel CAD parts and assemblies does require that the user follows the fundamental logic of the features. 

Solid modeling vs sheet metal modeling

The sheet metal feature in Onshape can be very counter intuitive, it looks like you are working on a 3D model, yet many 3D features are not working. Onshape is a solid modeler, but the sheet metal feature (in my understanding) is basically a 2D modeler. All features between 'sheet metal model' and 'finish sheet metal model' are applied on a 2D flat surface with no thickness, hence you can't apply extrude/add (adding thickness) but you can extrude/remove (punching a hole). It becomes a bit more intuitive when you edit directly in the flattend view.

Also note that after the 'finish sheet metal model' you are back in solid modeling space and all features you add to the part will not be present in the flatened view.

An example: a countersunk hole in sheet metal may require a 2 step aproach if you need the flatened view for DXF export: add a hole in the sheet metal part, finish sheet metal model, then add a countersunk hole feature. The flat patern will have the straight hole, the 3D model will have the countersunk hole. This may seem strange at first, but it makes sense in manufacturing; the sheet metal hole is punched or laser cut (2D), the countersunk chamfer is created later in a separate process (3D).

Yam_S

Hey john,
you wrote some interesting stuff, but pretty off topic in relation to the mirror.

I think that a feature mirror in sheet metal is too basic to be left behind these days.

eric_pesty

I forgot to add last time: if you are dealing with circular holes (which seems to be the case), you could look at using the hole tool as it will let you add many holes in different directions in one step (as another way to by pass the "mirror" issue).

Yam_S

The hole was just an example, the actual thing to mirror was slots in that case.

Speaking of the hole feature, its lacking "Symmetric" so much. a lot of times you have a good existing sketch for a hole, but it's in the middle of entities.

John_vd_Werff

Yea, I did got carried away a bit...

I agree that mirror of features in sheet metal should be possible within the same part. Mirroring features from a mirrored part back to the parent part like in your example..., I don't belive that would be good practice. 

Yam_S

making another mirror at the end of the design without disrupting the tree is just the right thing to do.
no need to look for different answers here, it should be possible.