How do I intersect two sketches on perpendicular planes such that they are aligned?

[mikejr83]

Hello,

I consider myself a CAD novice. This concept, in my head, is one of those things I figured is what CAD was designed to do.

I have a set of prints for a model airplane that I have digitized. I brought the prints into Fusion as canvases on the XY, XZ, and YZ planes. Then I calibrated them with some registration marks. Next, I sketched out the rudder section by "tracing" the canvas.

At this point I have a 2D, side representation of the rudder. The plans contain profile sections for rudder as a top view (XY) and fore/aft view (YZ). I believe these sections are drawn to scale in the plans (other non-scale sections have been explicitly noted) and their general area is indicated. For the curious, these type of cross sections are included so that the builder can match the profile of a surface. In the past I've cut these out from the physical plans to use as a guide during the sanding of the surface. I created sketches for both of these views so that I had a profile for each one.

Here's where I'm running into my issues. First, the image on each canvas contains all three of these views. This means that each of my sketches, when viewed in 3D space, are not even near each other. I haven't aligned the 3 profile canvases I created because, well, that is my main issue. How do I take these sketches and align them to give me intersecting sketches that a loft with rails can be made?

So, I figured the CAD software should be able to look at a path on a plane and "see" where points on a path of on an intersecting plane would meet. If my "primary" sketch was on the XZ plane I could pick some arbitrary Z height for a plane and then Fusion will tell me where the points would be located at the intersection. What I want to know is, given a constraint of the second sketch on the XY plane at what Z height would certain points intersect the other sketch.

My idea of the workflow is using the sketch on the XY as the selected primary sketch. I would then select points on this sketch to act as "intersection points". The sketch on the XZ plane would be the "tool". A "fitment axis" would be specified such that offset for the primary would be moved in that direction until the selected points intersected a path on the "tool sketch".

Another idea I came up with but do not know how to execute is to look at the XY and find the furthest fore point and measure to the aft most point, find the leading and trailing edge. With this measurement I could then go to the XZ sketch and find the "height" where the distance between the path representing the "front" and the path representing the "rear" was equal (such that this distance was measured perpendicular to the current plane). I could then create a plane that was through those two points and parallel to the XY plane. Then through some copy, paste, and move actions I could snap the profile to the two intersecting points. This seems error prone and time consuming, however.

[g-andresen]

Hi,

Please share a file and name the sketches involved.

File > export > save as f3d on local drive  > attach it to the next post.

günther

[wmhazzard]

First, you should align your canvas' to each other using the edit canvas command. Then create your first sketch. All subsequent sketches should have the relevant geometry projected into the current sketch. That will allow you to keep the sketches aligned.

[mikejr83]

@g-andresenhere is the exported Fusion file.

I'd really like to understand the correct way to do this.

@wmhazzard,

In my OP I mentioned that I cannot do this. The print has the three views on it. If I were to take, say the lower left corner of the JPEG, the coordinates 0,0, and place that at the origin for all three planes, XZ, YZ, and XY the canvases would be "aligned," however, the three profiles would be in different locations. The leads me to ask, how would I align three canvases to arbitrary points on the canvas?

[evanp4509U4JZ]

I do not know if this is the correct way but I would make each sketch a component, rather create a new component and start each sketch in it, and use joints to place them relative to each other. Do this by creating a component. Activate that component. Create the sketch within that component. Repeat for each sketch. Then use joints to align them.

[wmhazzard]

I would align the needed profiles of the canvas' to the origin and not the corners of the canvas'. Realign for each part. 

See model. 

[TrippyLighting]

Some of your ideas are misconceptions:

"More is better". That is the case. You use way too many spline fit points and by that I mean factor 10-20! That results in bad curvature.

[mikejr83]

So I see that you aligned the top view profile to the leading edge of the rudder where a point would coexist between the two. This is done at the "bottom" or Z "0". This places the trailing edge of that top view extending past the trailing edge of the side view. Now imagine you had the ability to "snap" the point from the top view to the path for the side view and then move the whole plane for the top view up and down such that the point traversed the path and "pulled" the canvas/sketch along with it. You could theoretically find a height of Z where the rear most point on the top view would come into alignment with the opposite side of the path so that now that front point was touching and the rear. Essentially finding where that horizontal "slice" came from. Doing this with a canvas would seem difficult as you are relying on your ability to visually see where this happens. If I spend a good amount of time tracing each view into sketches it would seem like there would be a way to calculate where this happens (given enough constraints).

[mikejr83]

I'll admit, I have no idea what I'm doing! 🙂

That was my general practice with using Inkscape to fit lines to make a vector image. I've tried reducing the number of points and using the "rubber band things" to make the curvature fit, but it seems to give me of a result that I wasn't happy with. The original plans may have been not done to traditional drafting standards, either. As I draw center lines and attempt at doing tasks like sketching half and then mirroring to make the sketch symmetric, I've found that the center line isn't in the center or the print was exactly symmetric to begin with.

My goal with the overall project, not just the rudder piece, is to teach myself CAD skills outside of just "make a sketch, make a different sketch, and now do a loft." I believe that I have certain simple tasks down. I figured with these plans I could use the views to learn more complex techniques and in the end be able to take the CAD model to make plugs or molds in order to make some composite parts. I've been following the Product Design Online videos over on YouTube and watch videos from another channel 3D modeling a jet. However, I'm having trouble applying some of those concepts when I get to my own projects.

[wmhazzard]

I aligned everything by eye. A canvas is not really meant to build a model from directly, measurements are meant to be used and the canvas is a guide. I guess that you don't have measurements to go by.  

[mikejr83]

I have the paper plans so I could measure based on them. There are registration marks with scale indicated on a portion of the plans. Something along the lines of "the center of this hole to the center of this other hole is 3 1/8in." There are two hashes where the centers are in the canvas. I've used that to calibrate each canvas that I imported. I viewed the canvases as I would if I was building the model by hand with wood. I'd work the wood till it met the outline of the shape on the plan, pin it in place, add the next one, glue, and then repeat. Similarly, I've used a sketch to perform the task of outlining the shape in that view that would meet the bounds of that outline. An over complicated way I thought about doing this was modeling each strip of wood that be used in the construction and affixing those bodies where they would be located with respect to the canvas. The issue that gets me to is how to make the compound curves that would be needed to shape certain pieces based on those profile views provided in the plans.

[TheCADWhisperer]

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@mikejr83 wrote:

Here's where I'm running into my issues.

1. First, the image on each canvas contains all three of these views. 

2. How do I take these sketches and align them to give me intersecting sketches that a loft with rails can be made?

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1.  You save the image several times - as many times as you have views.  Then crop out all extraneous views.

For example - if a sheet has a Top, Front and Side view - I save it three times named Top, Front and Side.

Then in Top file I crop out Front and Side.  Repeat as needed.

End up with image files with only one view in each image file.

Place these on canvas planes as needed and scale and align as needed.

(Make use of symmetry about the Origin as much as possible and practical.)

2. For sketching I use Project to connect a datum from one sketch to corresponding next sketch.

You should have started with a much more simple project rather than trying to fly this complex project which will likely result in either crashing and burning or in developing poor modeling techniques (habits which are hard to break).

Poor habits like using too many nodes in a spline.

The spline in the image below has only two points - a startpoint and an endpoint.

The curvature is controlled with the Handles. (Cyan glyphs at each end seen below.)

With Splines - Less is More.  For smooth curvature you want Fusion to interpolate the curve rather than trying to force a bunch of points.

In fact - as a beginner I recommend that you avoid Splines altogether.  Use Tangent Arcs instead.  These arcs should represent the splines within any possible manufacturing tolerance.

Here is one of your curves.

Edit your sketch and right click and select Toggle Curvature Display...

[mikejr83]

Ok I get the fact that I have a lot to learn when it comes to splines. I'll avoid them.

I still don't understand how to figure out where the horizontal slice goes in z position. I understand projecting the points onto the new sketch so that I can use them. All I'm reading is that you just have to "eyeball it" when it comes to picking where to put your plane. If it doesn't fit then change the offset. That seems not precise. It just seemed to me that I could make a sketch and get it as close to perfect and then find where it should fit in. I guess I'm so far removed from the correct way of doing things that the way I visualized solving this problem is not a concept in design/CAD.

At this point I'm frustrated enough at myself that I don't think I'll continue the project. It's looking like it is easier to destroy the original part making a mold than it is to make a model from plans and then make the mold.

Sorry.

[TheCADWhisperer]

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@mikejr83 wrote:

All I'm reading is that you just have to "eyeball it"

That seems not precise. 

... the original part making a mold than it is to make a model from plans and then make the mold.

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This drawing is art - not an engineering drawing.  I doubt it is very precise.  And it appears to be a photo of paper sheet  with some parallax error left to right.  Not even a good pdf original. 

If this were my project and I had access to original part - I would use a combination of the images (split up as I described earlier and actual caliper measurements of the original part to get as close as I can possibly reproduce in manufacturing tolerance (if I can't make it - there is no precision).

I would expect this to be a complex job and I have been doing this for 35 years (+8 more years out on the shop floor before entering the design office).