FeatureScript: Bounding Box Sketch

john_mcclary

Is there a way to create a bounding box sketch on the flat pattern view of sheet metal?

I need it for the stock size call out on the drawings, kind-of a pain in the arse doing it manually.

emagdalenaC2i

Here is a sample 

MBartlett21

@john_mcclary
@mahir
@emagdalenaC2C

Try out @Jake_Rosenfeld 's fs, which I have added flat pattern compatibility to: https://cad.onshape.com/documents/2ce3e64026df1ac7e63b98bd

MBartlett21

john_mcclary said:

That's cool, but it doesn't auto calculate the minimum stock size, and also does not allow you to insert the bounding box sketch into a drawing view

@john_mcclary
Please update to V 4.7, which adds auto-calculation to the feature

john_mcclary

Indeed it does,

Thank you all for your help, I will use the following workflow:

1) Use: V4.7+ of https://cad.onshape.com/documents/2ce3e64026df1ac7e63b98bd/w/7a2029e15b241c80c591a492/e/466a1aa41fce0c0be07f6436
2) Calculate Smallest on flat pattern
3) Create a secondary sketch and "Use" the result of featurescript
4) Insert into drawings
5) Win

emagdalenaC2i

well, actually the material and their density is set in a csv file... https://cad.onshape.com/documents/2718281828459eacfeeda11f/w/97628b48cc974c2681faacfc/e/6bbab304a1f64e7d640a2d7d
So, you can create a CSV reference parameter to read the material information ;-)

mahir

I don't know of a pre-existing featurescript that does this, but I would think it's doable. It's just a matter of querying all flatpattern geometry, getting a 3dbox around it, and using the 3dbox parameters to draw a matching sketch. I'm busy at the moment, but I wouldn't be surprised if someone wants to take this and run with it.

MBartlett21

@john_mcclary
Does it need to be a sketch? 

emagdalenaC2i

@mbartlett21 There are a FS "Calculate Bounds" that can create a bounding box of a part, but it don't work with the sheet metal flat part.

In the sheet metal flat view you only can create sketches

john_mcclary

mbartlett21 said:

@john_mcclary
Does it need to be a sketch? 

Yes, I need the sketch to be shown in the drawing view

emagdalenaC2i

Here is a sample 

john_mcclary

Oh wait, you just sketched it, thought you had a working FS ;p

emagdalenaC2i

Not yet

I am not sure... but I think we can't create a sketch in the Sheet metal flat view from a FeatureScript

emagdalenaC2i

Ok, It works...

In this picture the small rectangle is a sketch in the sheet metal flat view created from a FeatureScript ;-)


So now we only need to calculate the bounding box to drawn it in the sketch 

emagdalenaC2i

This is the initial code...

FeatureScript 847;
import(path : "onshape/std/geometry.fs", version : "847.0");

annotation { "Feature Type Name" : "SheetMetal BoundingBox" }
export const myFeature = defineFeature(function(context is Context, id is Id, definition is map)
    precondition
    {
        // Define the parameters of the feature type
        annotation { "Name" : "Plano", "Filter" : SheetMetalDefinitionEntityType.FACE && AllowFlattenedGeometry.YES, "MaxNumberOfPicks" : 1 }
        definition.myPlane is Query;

    }
    {
        // Define the function's action
        var sketch1 = newSketch(context, id + "sketch1", {
                "sketchPlane" : definition.myPlane
            });

        skRectangle(sketch1, "rectangle1", {
                    "firstCorner" : vector(0, 0) * inch,
                    "secondCorner" : vector(1, 1) * inch
                });

        skSolve(sketch1);

    });

john_mcclary

It's only creating a small square for me

emagdalenaC2i

emagdalenaC2C said:

So now we only need to calculate the bounding box to drawn it in the sketch 

Yes 
Step 1 - Create a sketch in the sheet metal flat view (DONE)
Step 2 - Calculate the bounding box (In progress)
Step 3 - Create the sketck (Pending)

emagdalenaC2i

One step further 

Now,
-Transform the sketch to be in the right position
-Change to construction geometry

MBartlett21

emagdalenaC2C said:

@mbartlett21 There are a FS "Calculate Bounds" that can create a bounding box of a part, but it don't work with the sheet metal flat part.

In the sheet metal flat view you only can create sketches

@emagdalenaC2C
I might actually makemake some improvements to it  

MBartlett21

john_mcclary said:

Oh wait, you just sketched it, thought you had a working FS ;p

Ps your question is now marked as 'accepted answer' 

john_mcclary

mbartlett21 said:

john_mcclary said:

Oh wait, you just sketched it, thought you had a working FS ;p

Ps your question is now marked as 'accepted answer' 

I break everything i touch >_>

MBartlett21

@john_mcclary
@mahir
@emagdalenaC2C

Try out @Jake_Rosenfeld 's fs, which I have added flat pattern compatibility to: https://cad.onshape.com/documents/2ce3e64026df1ac7e63b98bd

john_mcclary

That's cool, but it doesn't auto calculate the minimum stock size, and also does not allow you to insert the bounding box sketch into a drawing view

emagdalenaC2i

@mbartlett21 great work

@john_mcclary calculate the minimum stock size...
Are you talking about the optimization of the sheet metal

And, insert the bounding box sketch into a drawing view
Why you need that?

john_mcclary

Mostly for design review before release.
We look over all the details and if I did not show the bounding area of the part as shown below. Then someone asks "will that fit on a sheet?" (58 1/2" x 119") I can point to the "stock size" and say "Yes, We will have ~6 1/4" remaining, but we can only get one on a sheet".

And if i just add it to the stocksize on the detail callout note without dimensional proof on the part. Then it can slip through the cracks because Onshape will not let me add stocksize automatically to a custom property. So hand typed information needs a double check on paper.

emagdalenaC2i

You can edit the FS and add the stocksize properties to the part.

Also, you can edit the FS and show a message, or don't create the sketch if the size dono't fit on a sheet.

https://cad.onshape.com/FsDoc/library.html#module-properties.fs

john_mcclary

@emagdalenaC2C
Yes you can modify some pre-set properties, but not Custom properties.

emagdalenaC2i

You can use TITLE_1, TITLE_2 or TITLE_3 properties

john_mcclary

Can and should are two different things 

I used to do that trick before I had a company set up; mainly for the use of custom properties. So they are actually labeled to match their content.
It was a pain in the arse remembering which property "Title3" was really being used for "Mass"

On top of that I ran out of properties pretty quick what you see there is just the last 5 properties that are attached to every part, I was typing out the stocksize on the sheet manually then. I have it in a property in hopes Onshape will eventually let us FS-edit custom properties as well; at that point I will have the weight, stocksize, etc. all derived directly in the part stuido. (just like I did in SW)

brucebartlett

John what are you doing for weight ATM?  I really want a way to get these this automatically onto the drawing like I used to in SolidWorks as well. 

john_mcclary

Today I am just manually adding weight to the properties by measuring each part just before release.

But I have began attempting to make a featurescript to do this automatically by:
evVolume(context, { "entities" : definition.bodyQuery })

then reading the material property (I hope I can extract a density from this directly from the material library.... but I doubt it)

Then I was going to multiply them together and save the result in my custom property.

But luckily I look ahead and saw I couldn't save to a custom property, so I have up after getting the volume...

MBartlett21

john_mcclary said:

That's cool, but it doesn't auto calculate the minimum stock size, and also does not allow you to insert the bounding box sketch into a drawing view

@john_mcclary
I think it isn't recognising it as a sketch because of it being in a custom feature.
Maybe @lougallo could explain why.

P.S.
If you create a sketch then 'use' the edges, it can then be inserted into a drawing.

john_mcclary

mbartlett21 said:

john_mcclary said:

That's cool, but it doesn't auto calculate the minimum stock size, and also does not allow you to insert the bounding box sketch into a drawing view

@john_mcclary
I think it isn't recognising it as a sketch because of it being in a custom feature.
Maybe @lougallo could explain why.

P.S.
If you create a sketch then 'use' the edges, it can then be inserted into a drawing.

True, That would be a reasonable work around.

MBartlett21

john_mcclary said:

mbartlett21 said:

john_mcclary said:

That's cool, but it doesn't auto calculate the minimum stock size, and also does not allow you to insert the bounding box sketch into a drawing view

@john_mcclary
I think it isn't recognising it as a sketch because of it being in a custom feature.
Maybe @lougallo could explain why.

P.S.
If you create a sketch then 'use' the edges, it can then be inserted into a drawing.

True, That would be a reasonable work around.

And if you update the bounding box, it will update your sketch

MBartlett21

@john_mcclary
@emagdalenaC2C
I have made an improvement request for sketches created by custom features in the drawing view:
https://forum.onshape.com/discussion/9655/allow-flat-sketches-from-custom-features-in-drawings

MBartlett21

john_mcclary said:

That's cool, but it doesn't auto calculate the minimum stock size, and also does not allow you to insert the bounding box sketch into a drawing view

@john_mcclary
Please update to V 4.7, which adds auto-calculation to the feature