Projecting principal planes on sketch

[omkar.joshiT78SA]

How can we project the intersecting principal planes (XY,YZ etc) on the sketch? None of the project/include options  lets you select the plane, this is quite useful to get the horizontal and vertical references based on principal planes.

[wmhazzard]

In the sketch palette, select "sketch grid" and or turn on the origin in the browser. 

[g-andresen]

Hi,

Planes cannot be projected.
Projections or intersections are made from sketches and  solids or surfaces into a sketch, which is on a defined plane.

günther

[davebYYPCU]

Can you show why this is needed, Project > Intersect works.

Vertical and horizontal blue, orange and black lines can be dimensioned, purple lines from intersected planes can not, you have no control for that purple line length.

Might help....

[omkar.joshiT78SA]

I used to use Inventor earlier and it was very handy to quickly project the intersecting principal planes for horizontal and vertical reference. Project>intersect doesn't let me choose the planes, only geometric and sketch entities. Turning on the grid creates the reference however it doesn't constrain it by default (as it would happen if there were a projected curve).

[davebYYPCU · Accepted solution]

Project>intersect doesn't let me choose the planes,

Check my timeline, Project > Intersect Origin planes does work in Fusion.  I have no idea why you would want to.

Might help....

[omkar.joshiT78SA]

Thanks, yes just checked myself, the origin planes can be projected. It is very handy in constraining new curves/entities in the sketch. In below example, I was able to have reference of curve of projected plane to constrain the center of the right circle at the time I drew it. However, for the left circle, I didn't have any reference so its center remained unconstrained, and thus i have to constrain it as horizontal to origin as an additional step. Turning on grid doesn't automatically do this, unless I enable snap to grid, which I don't prefer.

[davebYYPCU]

It is very handy in constraining new curves/entities in the sketch.

Nope - you are limited to that short locked line for any advantage, as even you have demonstrated.

Draw a line and you can constrain the 3 circles and the Origin to it.

[omkar.joshiT78SA]

I was trying to demonstrate how projecting an intersecting (perpendicular) principal plane would be useful for quick reference and constraining. Yes unfortunately Fusion 360 projects a very small portion of the plane unlike Inventor, which automatically gages the overall sketch size and produces a line encompassing the whole sketch, which is what I wanted to achieve. 

[davebYYPCU]

Might work in Inventor, but useless in Fusion, there are better workflows.

[omkar.joshiT78SA]

Indeed, just need to get used to the best workflow possible with Fusion 360.

[stu_johnson]

Please show me your better workflow.

I have the same scenario. I want to constrain a circle vertically to the horizontal plane, but nothing seems to make it "stick". I have projected the plane and drawn a horizontal line as you suggest--which appears to be constrained, but cannot get the circle to constrain to the horizontal.

I want this:

[wmhazzard]

Delete the lines and projections, they are not needed. Place the circle near where it needs to be, select the horizontal/vertical constraint tool and place a horizontal constraint between the circle and the origin point, then add a dimension to fully constrain the sketch. 

[davebYYPCU]

Draw the circle, close to where you need it, with diameter dimension.

Make a horizontal dimension from sketch origin to centre point.

Make the centre point horizontal to the origin with horizontal Constraint, will turn the circle black.

Might help....

[stu_johnson]

I am trying to routinely "stick" circles to the horizontal plane as indicated below. I don't really know how I got the big circle to constrain, but I'm assuming it is because I projected the X-axis onto the sketch and then drew a construction line and made them all colinear.

But how do I extend those constraints to the other side of the vertical plane? Nothing seems to work.

[stu_johnson]

I am havving this same problem, except the Horiz constraint is not working for the left circle. 

in addition, I am trying to "stick" a sketch point at the intersection of the big circle and the horizontal plane in order to accurately dimension to the tangent. The Pick Tangent doesnt seem to work either.

[davebYYPCU]

You are working too hard, and contrary to popular workflows.

Start a sketch and hide the Origin planes, you will see a sketch Origin point.  Constrain to this point.  To stick to the x direction, use horizontal to this point.

Projecting the X plane, gives a purple short line that can not be altered unless you beak the link, so why bother, just draw your own horizontal line and it can be any length, and side you need.  You probably snagged the mid point of the projected line to constrain that circle.

Small circle, constrain horizontal with centre point, and sketch origin.

Pick Tangent is awkward in Fusion, Dimension > Select circle, right click, select pick Tangent, then select second circle right click, select Pick Tangent, and set distance.

Sketch points on circles for just Dimension, is clutter, and not required, the way Fusion works.

There is no wrong way, just better ways sometimes.

Might help....

[jhackney1972]

Both model Origin planes and Construction Work Planes can be projected into a sketch.  The Screencast will demonstrate.

[stu_johnson]

Thank you @davebYYPCU 

,

You got me unstuck. Very strange, "indirect" way of constraining, I must say. And I still needed to use a point to get the tangent-to-tangent to work, but the point snapped, so I got the constraints that I need.

Thanx for the help. It did...