Why can't I use construction lines in a sketch?

[JetForMe]

Why can't I use construction lines in a sketch? As soon as I do, it closes the sketch.

[NicolasXu]

Hi JetForMe,

I tried to make a construction line in sketch, and not able to reproduce the issue you mentioned. Please refer to the gif below for my steps.

Could you share more information about the problem you saw? A screencast would be very helpful for us to understand the problem. (http://screencast.autodesk.com/)

[JetForMe]

Here's my screen recording (the Autodesk app just hangs): http://cl.ly/1w2u3a3B0f11

It shows both the problem creating consruction lines in a sketch, seeing existing lines, and moving existing lines.

[NicolasXu]

Hi JetForMe,

Thanks for the screen recording. I understand the problem now.

In a word, in Fusion, sketch is a feature that can contain lots of sketch objects, and construction axis is not a sketch object but a feature which is at the same level as sketch. So it could explain why you see sketch exit when invoking Construct Axis command. (If you invoke Extrude command in sketch environment, you will see the similar behavior.)

To create construction lines in sketch for reference, we can create a sketch line, select it then toggle it to construction line from the Sketch Palette (or from the right clicking menu or pressing x key).

For another question of moving “construction axis”, in history-based modeling (the design we can see a timeline at the bottom of the application window), the construction axis is created based on the existing objects (edge, plane, etc.). Its position is determined by the specified objects so we cannot move it freely. When the consumed objects move, the construction axis will update automatically. If we stop capturing the design history (i.e. in history-free modeling), we can use the Move command to move it.  

The screenshot below shows how to convert a design from history-based modeling to history-free modeling. The command can be accessed from the right clicking menu of the root browser node. Because the history-based modeling supports parametric modeling, it's the defaule environment in Fusion.

[JetForMe]

I see.

In other CAD programs I've used, construction lines are very useful in the way they operate. First of all, it's often a simple gesture to create one (no need to choose it as a command), and with snap-to-feature support, makes it easy to get the construction line on a feature. But couple this with the ability offset the construction line in the plane, and it becomes incredibly powerful.

Is there no easy way to offset from a construction line (I don't mind making a new one) without switching modes? I don't mind that the construction is "tied" to a feature, but I do want to adjust where it ends up. They're much less useful without that ability.

[NicolasXu]

Unfortunately, in parametric modeling, we cannot offset the construction axis at present.

May I know what the purpose of creating the construction axes is? Is it acceptable if using the construction sketch line? In Fusion, we can create 3D sketch line by snapping to the existing objects, and we can copy/paste it and move the copy to anywhere.

Here is a screencast to show the steps. Probably it could be a workaround:

[JetForMe]

In my case, the profile in the sketch represents the part that I need to make. But there are holes perpendcular to the two angled sections. To drill those, I need to make a fixture that has the inverse profile with the angles and the curves, along with flats at the same angle to allow me to hold the work in the right orientation in the milling machine to make the holes. So, I was trying to offset the construction lines from the two angled lines to give me a guide for drawing the new profile.

[NicolasXu]

I see. Thanks for the information.

Another command might be useful is the sketch Project command. It can get the projection of the existing objects to the active sketch plane for reference. Furthermore, we can use sketch offset command to copy the selected sketch curves with a distance. 

Regards,

[JetForMe]

Actually, that brings up another thing I couldn't figure out how to do. I wanted to mirror a small part of the profile across a vertical bisecting line through the entire sketch. I had had created both a construction line and a plane, but I couldn't get the mirror command to work.

[NicolasXu]

Hi JetForMe,

Were you using the Mirror command under the Create drop-down list, or the Mirror command under Sketch drop-down list?

The former is to mirror faces, bodies or features instead of sketch objects. The latter is used to mirror sketch objects.

We can only use the mirror sketch command in sketch environment, and the source curves must be in the active sketch.

• In the Sketch drop-down list, click Mirror.
• Select the sketch curves to mirror. (Instead of the profile)
• Click Mirror Line then select the line to mirror across.

[JetForMe]

I don't want to change to history-free modeling, as it warns me that I will lose my entire history. Also, I use parametric modeling.

[JetForMe]

Switching between normal/construction is helpful, but I wish there was an easy way to make the line longer without changing its orientation.

[TrippyLighting]

Here, again, please provide a minimum in information. You looked at a computerscreen and likel had Fusion 360 open when typing ypur posts. Screenshots on a mac are exceedingly easy to do and the screencast tool provided as a free download from Auodesk could not be easier to use.

[jeff_strater]

Hi @JetForMe,

Reading back through this post, I think that there are some basic concepts that are not as clear as they could be in Fusion, combined with some unfortunate naming conventions that are the root of the problem.

I think the main misunderstanding here is the word "construction".  There are two separate concepts involved here, both which share that word.

construction geometry.  I prefer to call this "work geometry" (which is what it is called internally, but that's a different story).  There are 3 types of construction geometry:  work planes, work axes, and work points.  They are created using items from this menu:

These objects create separate items in the timeline:

And create items in the browser:

as you can see here, the origin items are also composed of construction/work geometry.

construction/work geometry can be used in creating modeling features.  You can create a sketch on a work plane, you can use a work axis in the Revolve feature as an axis of revolution, etc.

sketch construction curves.  As you know, sketch is a little island of functionality itself.  You create a sketch, you edit a sketch, while you are in sketch mode, your focus is creating and editing items in that sketch.  Sketches contain curves (including lines), points, constraints, dimensions, text, etc.  A sketch does not contain work planes, work axes, etc.

Within the sketch environment, a sketch curve can be a "construction curve".  This is just an attribute on a curve that changes its appearance and, to some extent, its behavior.  The construction attribute of any curve can be toggled using the sketch palette when a curve is selected:

or by right clicking and choosing the "Normal/Construction" command:

When a sketch curve is marked as construction, its appearance is changed to dashed:

And, sketch construction curves do not particpate in profiles, paths, etc in features.  That is why, in the above picture, there is no shaded region that can be extruded.  That, in fact, is the main reason why sketch construction curves exist - to limit their participation in consuming features.  In every other way, these behave identically as "normal" sketch curves.  You can dimension and constrain them identically, etc.

The last concept that is probably relevant, as @NicolasXu mentioned is "Projected Geometry" in a sketch.  The Project command allows you to project the geometry from other objects into the sketch.  You can project model edges, sketch geometry from other sketches, or work/construction geometry onto the sketch plane.  The "Inculde 3D Geometry" allows you to bring arbitrary 3D geometry (including work/construction geometry) into the sketch world as 3D objects, where they can be referenced.

So, with these two concepts defined (and hopefully my definition is adequate), can you re-state your question?  What is it you are trying to achieve?  I believe that whatever it is, most likely there is some way to do it in Fusion.  We'd be glad to help illustrate it.

Jeff Strater (Fusion development)

[Anonymous]

SLOW DOWN when demonstrating these things.    I am sure  you have done this so often it's second nature to you,  but there is no way in heck a newbie can follow your lighting fast demos, much less take notes.