Techdraw: Dimensioning an Ellipse?

[AzAv8r]

I have recreated a cam design in FreeCad (19.4, Windows 10), and have created a technical drawing of it with the wonderful TechDraw workbench.

The cam has one elliptical arc, and I am trying to figure out how best to dimension that arc. Techdraw doesn't like it (more in a moment), although it would seem I should be able to use cosmetic annotations for this purpose. So I'm hoping someone can give me some suggestions.

A Google search doesn't provide any "standard" way of dimensioning an ellipse, and generally just returns construction methods. Sketcher works just fine, so I don't need those.

An ellipse is defined by four data items:
- a center
- a major axis
- a major radius
- a minor radius

So what I'd like to do is place an arrow from the center along the major axis, and then label it with the two radii. If the major axis was not horizontal or vertical or clearly defined by some other geometry, I'd also want to have the angle of the axis indicated.

To illustrate what I've got, I snapped two images: one of a version of the cam which uses an arc in lieu of the ellipse (since this shows the radius dimensioning arrow), then a second image with the elliptical arc. (They do have 10 thou chamfers on the corners which are not yet dimensioned; I'm assuming those are best dimensioned with a note.)

The cam is constructed from a sketch with three concentric circular arcs, an additional concentric arc which is either circular or elliptical, and two pairs of arcs each pair of which is symmetrical on the horizontal axis, and tangent with other geometry. I created both a top and bottom view for dimensioning due to the number of arcs to be dimensioned - this lets me distribute those dimensions across a larger area (with fewer features) for clarity.

First, the circular arc version. The arc of interest is in the top view, of radius 0.4750". In this case, it is circular, and I've aligned the radius vector horizontally (which is how I'd want to do it on my ellipse.)

Screenshot 2022-06-09 155041.png (58.85 KiB) Viewed 2098 times

Next, the elliptical arc version. Here again, the arc of interest is on the top view. It IS dimensioned, but it has a value of zero and the arrow is oddly placed. I got a dialog box saying the arc is a bspline and an approximation would be drawn. However, I then got an error, which resulted in an oddly-placed arrow and the zero dimension. As described at the start of this post, I'd like to insert (and label) a cosmetic arrow from the center point to the arc and add labels. Is there a way to do such?

Screenshot 2022-06-09 155458.png (48.24 KiB) Viewed 2098 times

A couple of other oddities in the drawing with the Ellipse, both on the top view where the ellipse is present:
1. The bottom radius of 0.03125 has dimension line connected at an end of the center marker. All the other ones are okay, and the dimension is correct.
2. The chamfers on the thin part of the cam did not work in PartDesign. A dialog box popped up which said "failed to create chamfer".That is the reason they do not appear in the drawing.

A few other TechDraw questions, while I have your attention...

1. Is there a way to force alignment of stacked views like this (so edges were aligned)? So for example the right edges of the model in all three views were aligned.
2. Similarly for dimension errors - is there a way to fix or bias dimension offset spacing so I can easily snap-to an appropriate dimension and equally space length dimension lines? So for example, in the bottom view the vertical dimensions 0.3125 and 0.6250 could be at equally-spaced offsets from the model (say, 0.2" offset and 0.4" offset), and that in the middle view the 0.292" vertical dimension was aligned with one of the two in the lower view.

I'd also welcome any additional tips / best-practices that my drawings would suggest I could benefit from.

Thx,
Jon

[Shalmeneser]

File ?
Full version ? (Follow link in the red banner above)

[Workshop_Notes]

Some of it is a problem with terminology. 'Radius' has a very specific meaning in mathematics (https://en.wikipedia.org/wiki/Radius_of_curvature). The unique feature of a circle is that its radius is constant for its entire perimeter. The radius is also a property of the circle object that is stored in the model database, so is easily retrievable.

Clearly, the (mathematical or instantaneous) radius of an elliptical curve will very around its girth.

When defining the elliptical curve as you do, we choose to use the term 'radius' in a different way, for four very specific points on the ellipse, the ends of its major and minor axes. And when we use 'radius' there, we mean the radius of the _circular_ arc that when struck from the centre point of the elliptical curve will intersect the axis at a point on that elliptical curve. At those points, the centres of the circles and ellipse coincide but the radius of each curve differs.

Thus dimensioning the true radius of an ellitical curve at any specific point, even a specialised one like the end of one of its axes, is more complicated as the ellipse object will not be stored in the database in that form. Hence the radius dimension tool (by design) just may not have enough inbuilt smarts to work properly on anything but a circular object.

I do not know if you can overlay a helper rectangle of the major and minor axis dimensions and dimension that using a linear dimension tool, using 'R' as a prefix in the dimension text format. Even if you somehow get a correct number at the point you want, form your own definition of an ellipse, that single dimension plus the centre location does not fully define the ellipse, even if you add 'elliptical arc' as a note.

What is the purpose of the drawing? If it is to send out for manufacture, does the machine that will grind it understand elliptical arcs? There is no G-code to my knowledge for this, so at some point in the toolchain the curve will be converted to either straight lines or circular arcs.

[Shalmeneser]

(Center Marks don't work ?!)

[papyblaise]

if you use the Fc tool for creating ellipses, it makes you a mathematical B-spline, with all the disadvantages of B-splines: chamfer or radius failure, connection with other curves, impossible dimensioning
If the "old-technoligic" construction of the elipse is enough for you, you draw it with 4 arcs of a circle and the rest is easier.
If you have a good idea of these arcs although created in the B-spline version, you can dimensioning them using a label with a leader line

[AzAv8r]

Version:
OS: Windows 10 Version 2009
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24267 +148 (Git)
Build type: Release
Branch: Branch_0.19.4
Hash: 476ecf091941bead59b14e44afa6064d5a66afa3
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.3
Locale: English/United States (en_US)

I understand the use of the b-spline as an approximation, and this is the reason I expected to need to create a cosmetic dimension.

The purpose of the drawing is to convey to someone who wants to reproduce the cam manually the geometric constructs which produce the shape. (It's not an assembly drawing, and it's not an input to CNC except through another human designer.) I have made available STL (from OpenSCAD) and STEP (from FreeCad) for someone who just wants to produce the design in that form. But others want to machine ii or program it themselves; thus the desire to produce a dimensional drawing.

In OpenSCAD, the ellipse is produced mathematically - differentially scaling one axis of a circle: scale([1.25,1]) circle(r=dw/2);

On the center marks for arcs: they work, you just have to turn them on. It took me a bit to find those. You'll need to do it for each view where you need to dimension arcs. Select the View in the TechDraw page, then on the "View" tab scroll to the "Decoration" group and set "Arc Center Marks" to TRUE.

Both files are attached. "...v4rad.FCStd" is the version with a circular arc, "...v4a.FCStd" is the version with the elliptical arc.

[AzAv8r]

(Center Marks don't work ?!)

That'll work, thanks! And there's a lot of new stuff in there I'll need to figure out.

I don't see the "Arc Center Marks" Boolean in the views.

[Shalmeneser]

I don't see the "Arc Center Marks" Boolean in the views.

The Marks box is not in the TechDraw_ProjectionGroup but in each view of the projection.

(The marks were not visible in my other computer.)

[papyblaise]

with the new tools from Techdraw, it should do it

[Workshop_Notes]

if you use the Fc tool for creating ellipses, it makes you a mathematical B-spline... ...If the "old-technoligic" construction of the ellipse is enough for you, you draw it with 4 arcs of a circle and the rest is easier. If you have a good idea of these arcs although created in the B-spline version, you can dimensioning them using a label with a leader line

Going from end to beginning of the quoted post above:

1) The term 'good idea of these arcs' kind of implies guesswork. If you know the major and minor axis lengths of the ellipse, a proper geometric construction of the 4-arc approximation (that will give dimensionable radii and centre points and tangency at arc end points) is easy. See: https://www.had2know.org/makeit/ellipse ... r-arc.html

2) I wonder if it would be useful to add a 4-arc approximate ellipse to the available drawing tools as a companion or alternative to the B-spline version. From a manufacturing/engineering point of view circular arcs are much easier to make.