What is the best way to offset vectors depending if they're positive or negative?

Lee_Hesketh

Hello all, I have come across a peculiar error in my code. I am using a vertex as a reference point for the first corner of an skRectangle(). I am using worldToPlane() to achieve this. I am then adding a vector which is offsetting the first corner in relation to the vertex. It looks like this:

skRectangle(sketch1, "rectangle1", {
                        "firstCorner" : worldToPlane(evPlane(context, { "face" : comps.sketchFace }), comps.vertexPoint) + vector(h, -v1),
                        "secondCorner" : worldToPlane(evPlane(context, { "face" : comps.sketchFace }), comps.vertexPoint) + vector(h + width, height)
                    });

I am making h and width positive or negative by using the reference point and the centre point of the face, as seen by the two red dots. I am doing this by adding the difference in x coordinates and the difference in y coordinates. R = reference point, C = centre point

if((R[0]-C[0])+(R[1]-C[1])>0)
    {
      h*=-1;
      width*=-1;
    }

Since this featurescript will be used on parts such that the face shown is aligned with either the X or Y axis, that is why I am adding both X and Y coordinates. For example, in the picture, the Y coordinates of R and C are equal since they are on the same plane. This means that (R[0]-C[0])+(R[1]-C[1])
is the same as R[0]-C[0]. If this value is greater than 0, R is more positive than C and therefore h and width should be negative. And so to the error. I debugged h and width and they are indeed negative. However, the resulting geometry, the red part labelled Tenon, is going the other way and I don't know why.
Could anyone either explain what I'm doing wrong or suggest an alternative to achieve that same thing?
Document:https://cad.onshape.com/documents/580b256ade95e210af0261d8/w/1d22e17d9b07548059b7b311/e/119330903d9f0efa384481b9 , "Mortice and Tenon"
Thanks
Lee Hesketh

billy2

Lee-try this

I want to draw on this face highlighted below:


To create a sketch, use this vector to offset the sketch:


Use the face normal for direction, this is the sketch Z direction and
also called the sketch normal:


Use this edge to orient the X axis on the sketch:


This creates a sketch where the bottom left corner is 0,0 and the axis are aligned properly:


Now it's pretty easy to position the sketch rectangle. Just extrude it, the face normal set the sketch up so positive comes out of the part.

If you're going to use sketches, use the 3 vector method and position the sketch properly. You shouldn't have to think about the math or abs(X) or any of that stuff. 

billy2

Lee-

Was poking around in your code. I have no solutions to your problem. Just some observations.

1st-
change part studio units to meters, it makes debugging this stuff much easier. You can use the measure tool and see which coordinate system your comps object is using.

2nd-
 I have no idea what this is initialComputations(context, id, definition); I checked documentation and found nothing. What's it returning?

With units set to meters, I can understand comps object:

Trying to find something meaningful in comps object:

            debug(context, comps.mid.maxCorner);

            debug(context, comps.midPoint);

            debug(context, comps.mid.minCorner);

            println(comps);

I don't like comps. Seems useless to me.

I don't trust this at all because of the comps query, shouldn't have to compute h or width:


Can't you query the face or edge and get better properties?

comps is some kind of 3D object I'm assuming it's the body of your face query. I did probe it looking for some meaningful data. centerpoint & centerpoint2 are useless. centerpoint of what?


I think you're barking up the wrong tree with comps. I'd look for a better query. The math should work itself out once you get good a query.

billy2

pretty print

Onshape can you please give us a function that prints an object in an indented format?


I feel like I'm being punished for something when viewing an object.

Lee_Hesketh

Ah, I should have explained. initialComputations is just an arbitrary function that I need to calculate the width of the part so I can use that as the value for the width of the tenon. I am then using that as an editing logic function. However, the variables need to calculate part_wide are also needed in the main body. So I added all of the variables to a map called result.

Comps is just a variable that calls initialComputations so I don't have to retype the whole thing. So when I want to get say vertexPoint, since it is in initialComputations, I call it by using comps.vertexPoint. When you printed comps, you printed the entire map.

CentrePoint 1 and 2 are the centres of the two end faces, in this case, the faces that are in the XZ plane. I need centrepoint1 because I am using that to determine if h and width should be either positive or negative. Both centre points are need later on when creating the mortice. I am using them to find any parts that contain those points. They are hidden in the part studio, but these are the targets that I use when performing a Boolean operation with the tenon.

H and width are not calculated, they are values the user inputs, width and horizontal offset.

The problem still remains. If you unsuppress mortice tenon 2, you will see that it works as expected. It only doesn't work on parts perpendicular to it and I don't know why.

billy2

vertexPoint is world coordinates:


maxCorner equals vertexPoint and is world coordinates:


minCorner is world coordinates:



I'm going to stick my neck out and say that initialComputations() is returning world coordinates.

Lee_Hesketh

Yes it is, but I am using worldToPlane(). Is there a better way of doing this? How could I return plane coordinates?

billy2

This is the h & width stuff that I'm not sure about:


Seems like if it's set up properly, you shouldn't have to worry about direction.

Below, the sketch creation scares me. I don't think you have control over the sketch transformation OS is returning and could be flipping horizontal & vertical. I'd feel more comfortable defining this sketch with 2 vectors and removing the ambiguity. OS uses some patterns to generate sketches (as far as it's transformation is concerned), but I'm not sure you can rely on it consistently. Will horizontal always be to the right and vertical is up? I don't think so. Width & height are based on horizontal & vertical?





I'll look at your working example and see if the newSketchOnPlane composition is the root of the problem. This seems ambiguous to me not sure I'd rely on it. Without knowing horizontal & vertical I don't think width & height make sense.

Lee_Hesketh

I still think I need to determine direction. I'll link you to another of my posts that addresses this.
https://forum.onshape.com/discussion/5184/vector-coordinates-help#latest

billy2

There were many that tried to create Mortice & Tenon features in the beginning of featureScript. A school had many students working on it. Did you look at their code?

If I were going to write one, I probably wouldn't use any sketches. I was thinking you'd need the inner & outer edges shown below & a tab length:


From here I'd create some sheets:


Then work some magic:


I don't think I'd dance through a bunch of sketches and create mortice tenons as if building it with the user interface.



It'd be cool to mortise & tenon this:

Lee_Hesketh

That's not a mortice and tenon though. This is:

billy2

This is indeterminate (no answer):


This is determinate, but I have another piece of info (rectangle center):


But what's X or Y? Is it +X or -X? Depends on which quadrant you're in. It's based on the transformation they used to get you into a sketch. 

I think you're going to have a real mess on your hands keeping all this straight.

Lee_Hesketh

That's why I need to determine if h and width should be negative. If the corner coordinates are greater than the centre of the faces, then they are negative, since otherwise I'll be adding a positive offset which will result in the geometry being outside the part. I have changed the code slightly. I am now creating a plane with vertexPoint as the origin, the face I am creating the sketch on's normal and an x direction of (0,0,1), since the Z axis is used for both orientations. However, the error still remains. H and width are negative and they should be, but it still appears to be adding them, not subtracting.

billy2

Ok, let's forget about featureScript for a moment.

I'm using the user's interface.
-I've created sketch 10
-I have no idea what horizontal and vertical are, but who cares
-I've worldtosketch these points so now they're in sketch10 coordinate



So you know
-vector p2-p1


You also know
-vector p3-p1
 

These are the same vector direction, so p3 is useless to you


You need p4 and you need to know that's it's the width:
-unitize(vector p4-p1)* width, here's your width


From p4 you can get p5
-unitize((p4-p1 cross with Z) cross with (p4 - p1))*height, using a triple product



I don't think you can get p4-p1 from your query. Your problem is indeterminate.

To get the extrude direction you can ckeck the dot product between the sketch normal and the face normal possibly returned in comps.

sketch10 width & height are meaningless unless you compose the sketch transformation using p4-p1. If you know p4-p1 then screw the composition of the sketch transformation and perform the vector math in sketch (width & height won't match vertical & horizontal).

My point, without knowing p4-p1, can't solve the problem.

My point about in/out of sketches is that it's a nightmare keeping it straight.

Let me know if you get it working,

billy2

centrePoint1 & centrePoint2 are the centers of the extruded faces. Where's the center points for top & bottom extrudes? What if I extrude a hex?

centrePoint trying to understand why it's not centerPoint,

Did you write initialComputations() or did OS?

Lee_Hesketh

Well my code already gets p4 so p4-p1 is easy. I think I may have not explained fully. This is the face that I am creating the sketch on.
So the normal to sketch 10 in your example is the Y axis. In my picture, the red part should be inside the yellow part like this.
To achieve this, I have entered in a horizontal offset of -15mm. Which essentially, if the code worked correctly, is a 5mm offset and a 10mm tenon width. This is a workaround but I want it to work first time.

Lee_Hesketh

Regarding centrePoint, I'm British and that's how we spell it. And I wrote initialComputations. Also, this script is only for use on cuboids and will only extrude rectangles.

billy2

To get proper direction, go the opposite direction of the face normal and go in the direction of p2-p1 in  your current sketch. 

My fear is that you'll get it working for this case, but when you spin the part around to the back side and try it, it'll be wrong.

I'm not sure all this will be robust enough to work all the time.

billy2

This seems trivial. Pick a face, match tall face edge with width & short with height. Not sure this is always correct.



Are you automatically going to find the mating part or does the user pick it. Is it 1 sketch that cuts /extrudes or 2 sketch transforms with each part getting it's own sketch? If you use 2 sketches, remember you have to go from sketch1 to world and then from world to sketch2. There is no from sketch1 to sketch2.

This one seems more trivial than the mortice and tenon.

billy2

So a plane is typically declared by it's Z direction. Then you need to supply the X direction to orient.

I think in CAD they'll ask for X and then Y. Y doesn't have to be orthogonal X.

I've never created a sketch based on 2 vectors. Hopefully you can. It seems to me, sketches defined on faces use the minimum number of translations. If you looked normal to sketch10 and it's origin, that would match the world origin. The rotations are magic. There's multiple solutions and which ones they have chosen to create a sketch on a face, I'm not sure.

A triple product does all the magic.

Triple product is:
Z crossed with X -> gives you Y
Y crossed with Z ->gives you an orthogonal X

Triple products give you 3 orthogonal vectors. A coordinate system, sketch, circle......

billy2

You don't need a sketch to extrude:
-pick some 3D curves and extrude this way along this vector. opExtrude doesn't have a sketch dependency. 




Here's your sketch based on 2 vectors:
It actually takes 3 vectors.

I think a triple product is easier.

billy2

Here's the code to create a sketch anywhere @ orientation:

annotation { "Feature Type Name" : "sketch" }
export const myFeature = defineFeature(function(context is Context, id is Id, definition is map)
    precondition
    {
        annotation { "offset" : "My Query", "Filter" : EntityType.EDGE, "MaxNumberOfPicks" : 1 }
        definition.offset is Query;
        annotation { "normal" : "My Query", "Filter" : EntityType.EDGE, "MaxNumberOfPicks" : 1 }
        definition.normal is Query; 
        annotation { "x" : "My Query", "Filter" : EntityType.EDGE, "MaxNumberOfPicks" : 1 }
        definition.x is Query;
    }
    {
        // println(
        //     evLine(context, {
        //             "edge" : definition.offset
        //     })
        //     );
        
        println(evCurveDefinition(context, {"edge" : definition.offset}).direction);
        println(evLength(context, {"entities" : definition.offset}));
        
        var offset=vector(evCurveDefinition(context, {"edge" : definition.offset}).direction)*evLength(context, {"entities" : definition.offset});
        var normal=vector(evCurveDefinition(context, {"edge" : definition.normal}).direction)*evLength(context, {"entities" : definition.normal});
        var x=vector(evCurveDefinition(context, {"edge" : definition.x}).direction)*evLength(context, {"entities" : definition.x});
         
        println(offset);
        println(normal);
        println(x);
        
        var sketch1 = newSketchOnPlane(context, id + "sketch", { "sketchPlane" : plane(offset, normal, x)
            });
        
        skLineSegment(sketch1, "line1", {
                "start" : vector(5, 0) * millimeter,
                "end" : vector(50, 0) * millimeter
        });
        
        skLineSegment(sketch1, "line2", {
                "start" : vector(0, 5) * millimeter,
                "end" : vector(0, 35) * millimeter
        });        
        
        skSolve(sketch1);
        
    });

Lee_Hesketh

I've got it close to working, I didn't need to calculate h and width, just set the planes' x to C-R. The only thing now is the planes' z. It is either +z or -z. How could I specify it to use the positive Z axis. I tried creating a coordinate system which worked, but the plane is in the XY plane, not XZ or YZ. Could I just rotate the plane? If so, how?

billy2

Lee-try this

I want to draw on this face highlighted below:


To create a sketch, use this vector to offset the sketch:


Use the face normal for direction, this is the sketch Z direction and
also called the sketch normal:


Use this edge to orient the X axis on the sketch:


This creates a sketch where the bottom left corner is 0,0 and the axis are aligned properly:


Now it's pretty easy to position the sketch rectangle. Just extrude it, the face normal set the sketch up so positive comes out of the part.

If you're going to use sketches, use the 3 vector method and position the sketch properly. You shouldn't have to think about the math or abs(X) or any of that stuff. 

Lee_Hesketh

Yeah, I am using a similar method. It does create sketches but sometimes in the wrong direction as you can see.

This is what the plane should look like all the time. However.

Sometimes, the third axis that isn't the x or normal points the other way. How could I set it such that the plane looks like the first one all the time? Also, what do you mean by offsetting the plane? 

Lee_Hesketh

@billy2
I have managed to get my script to work now! I simply inverted the variables controlling the height of the tenon if the z coordinate of the cross of the x and normal was greater than 0. Thank you very much for your help and persistence, I finally understand why my script wasn't working in the first place thanks to you. Keep up the good work!

billy2

I'll keep cross x with normal in the back of my mind when using 3 vector sketch method. Seems like it should be deterministic on it's own without that check.

Thanks for the problem, I've been meaning to figure out sketches in featurescript. I think I too can create geometry with sketches now.

 When you're done with your script, take a video and show me how it works.

Cheers!