I've created a sketch ontop of a body (lid) I'm making. I used the "Horizontal/Vertical" sketch tool to center it but now I want to set the measurement to be, for example, 10mm in from the sides and perhaps 55mm from the top/bottom:
How would I do this?
Thanks!
Hi @Cowski,
You should be able to do this just using the sketch dimension command. Here is a screencast:
Jeff
@jeff_strater Something I have noticed is if you don't have Autoproject edges on references turned on you wont be able to do what you did in your vid unless you project the edge's in or popped it on it's side and did a 3D sketch. If a newbie does not know that it may be a problem, anyway it would make a good subject for a vid.
@Cowski sorry for highjacking Iam just highlighting this.
Yes and no. In my video, I sketch directly on the face, so those edges are included in the sketch, which is controlled by another option: "Auto project geometry on active sketch plane". In your settings, I see you have that turned off. So, in your case, yes. If that option is turned off, then turning on "auto project edges on reference" will be needed, or manually projecting the edge into the sketch.
Jeff
just to follow up a bit more on the topic that @daniel_lyall brought up. Daniel is correct in what he said. The situation is much more complex than I described. There are a number of factors involved in projecting model geometry into a sketch. So, just in the interest of anyone who is watching this thread, I'll try to describe it. To be honest, though, I am not happy with this amount of complexity, and I wish it were all much simpler.
The main point is, as you bring up in this thread, sometimes you want to constrain or dimension to edges or faces in the model. There are several commands, under the Sketch -> Project menu that allow you to bring some form of model geometry into your sketch. These commands cause an explicit action to occur. For instance, the Project command allows you to select an edge and project that edge into the current sketch plane. The Project Intersection command allows you to create sketch geometry at the intersection of the selected object and the sketch plane. And so on. So, you can do these projections manually using these commands. This is how I prefer to work.
However, people objected to this way of working, because it requires too many clicks. So there are two options that control what we call "auto projection", which can streamline this process. The first is called "auto project geometry on active sketch plane". How's that for a concise option name? This option controls whether Fusion projects the edges of the face, if you sketch on a planar face. This is a fairly common option to want to be set. If you sketch on a face, you often want to dimension to the edge of that face, as in your example. However, though those curves are indeed projected into the sketch, Fusion does not draw them. Why? Well, some people complained that the sketch looked "too busy" when we were drawing them. So, we turned them off. You can still dimension to them, you just have to find them.
The next option is called "auto project edges on reference". This command allows you to project edges that are not on the face that you sketched on. So, if you have a body, and are editing a sketch, you can just snap a line endpoint to a model edge, and Fusion will automatically project that edge into the model. But, there are some conditions. You have to be looking right straight at the sketch ("auto look at sketch"), and you have to be in orthographic views, and you have to have "3d sketch" turned off in the sketch panel. But, this can be useful if you don't want to manually project model edges. This is the option that Daniel was referring to.
Hopefully that is clear, or at least somewhat. It is complex, I know...
Thanks,
Jeff
