add relations fix questions

[Petertha]

I've imported a DXF from a 2D export. In hindsight this should have been obvious what was going on, but I started drawing my own construction lines within the sketch to evaluate things. Like is this feature symmetric to that feature, or is that point horizontal to that line...etc. But because the entire import was blue (unconstrained) I managed to distort some of the original sketch because it was unconstrained. So now I decided to fix the relations so they are locked down, at least as far as they relate to one another. And I think this is a bit safer state to copy/move them to other construction planes

Anyways, once 'fixed', the lines & entities turn black as expected. But inevitably there are some remnant blue dots in there. I can't physically move them. What does this mean to SW? Why wouldn't everything be black since I've selected everything within a window & its all on one layer?

[DanPihlaja]

When you are in 3D, when you "Fix" a line, the endpoints are still free to slide along the length of the line. You would ALSO need to fFx the end points if you wanted them locked.

This same behavior is is represented in the drawing side of things as well. However, since the drawing side of things was NOT intended with sketch elements in mind, they are less robust (in my experience).

In my opinion, you should bring the entire DXF into a sketch at the part level. Fix what is needed, and make your edits. Then you can bring the sketch into a drawing and print it out as needed.

[Petertha]

You touched on some things I'm still struggling with a bit & the reason for these workarounds. When I go through the import wizard to bring in a DWG file, I assumed I could prescribe which SW plane to align it with using the drop down selection. But it always seems to place it onto SW Front View. In order to build my 3D model, I copy-paste elements of the DWG onto my particular SW plane & align the elements to the origin. That's where I have to be careful because when initially pasted, the original relations are kind of flexible in this state. If I draw reference lines or whatever to some features to help with alignment, I can unwittingly distort them. It would be better if I could import the entire DWG file into Top view, align & delete what I don't need, then repeat for Right & Front Plane. Whereas now I am using the default DWG import plane view as my copy-paste source. Hopefully this makes sense. Maybe there is an easier methodology to what I'm doing.

[Petertha]

I was hoping this is where I could define the destination SW view to place the DWG but it seems to have no effect? It always comes into SW Front View

[SPerman]

If I were going to do this, I would do it in the context of an assembly. The top level assembly exists only to help with the relationships between the sketches and the finished part.

Part 1 would be the "reference" part. In here I would import the sketch (or sketches) that I needed to use as a reference.
Part 2 would be the part I am actually working in.

Import part 2 into the assembly and lock its origin to the assembly origin. Import part 1 and put it wherever it needs to be. If the DXF imports into the reference part on the top plane, but you need this plane aligned to the front, this is where I would do that.

From there, I would duplicate the "reference" sketch in the "Part 2" part using "Convert entities." I would not ever touch this sketch, it is also for reference only.

At this point I would delete the relations to the original "reference" part sketch, and the assembly can be deleted.

Finally, back in the working part, I would create another sketch. This one is the sketch I would make the actual changes to. The previous sketch is always there for reference, if needed.

Hopefully this makes sense.

[CarrieIves]

I would bring in the DXF and not worry much about which plane it puts it on.

Turn on the 2D to 3D toolbar.

The first thing I would do is then edit the sketch to get rid of any notes or drawing format stuff if that came in.

Do you have different things on layers in the DXF? They can each be brought in as separate sketches.

I would then copy the sketch and paste it either to the front plane or a different one so if I make a mistake I have a copy.

In the 2D to 3D toolbar, when you are editing a sketch, you can select items and then tell it what plane to put them on. There are other buttons for aligning sketches, but I haven't figured that out yet.

I then would create new sketches and copy the sketch segments I want to that sketch using convert entity, then remove the convert entity constraint and constrain it the way that makes sense. I would use "fully define sketch" to help with assumptions like horizontal, vertical, and tangent.

Good luck.

[Petertha]

Thanks for replies. Hopefully the end result will add some context. The task was to 3D model this piping system based on partial datum references sketched in the source 2D DWG file. I first needed to select the necessary pipe entities DWG & copy them into my 3 primary planes, preserving their dimensional relationship & aligned to a common reference point. Thereafter each 3D pipe segment was modelled a bit different depending on the shape itself. A few segments were simple sticks orthogonal to one of my primary planes, which were easy. Several others had to be generated in 3D by projecting 2 separate sketches to one another, or to an intermediary plane & further referenced. For non-coplanar pipe segments I made the curved elements using a 2-point spline, constraining tangency to each segment end & that seemed to make decent 3D curves. After the piping was done I just copy pasted the 3 engine views in position for visual sanity check.

So I never really had a 'part' to copy or superimpose the source sketch to, which is what some of those commands require to work. I just had my 3 primary planes to begin. Turns out copy-paste was about the most expedient way to get it plopped onto my plane, translate into origin position by dragging a known reference point. Then immediately fix relations so it cant inadvertently move. Then yes, I left those layers alone & made my own layers to proceed with pipe building

Regarding the suggestion to use an Assembly template, I'm not quite understanding what benefit that would provide. Now that this particular job is hopefully illustrated a bit more, can you expand on that? Do you mean make a dummy part (as opposed to a plane) just as a more expedient way to copy over the source sketch elements (like using Derived Sketch for example).

[Petertha]

Well I don't know what I was doing incorrectly before, but it turns out I can use Derived Sketch function to copy/transpose a sketch to any other plane, thus creating a new sketch. I was able to transpose to a part face but that's just an additional capability. When its first inserted to the target plane, the entities are all blue (undefined) because the group is not yet referenced to an origin point or whatever. However it does preserve the sketch entities between each other, kind of like a group. You can lock the sketch into a desired position by dimensioning or alignment. Where I was getting confused is the new sketch does not then turn black indicating fully defined. But I think that is SW way of saying its not, really. Because if the source sketch changes, then the derived sketch updates accordingly. Totally useful. This method saves some copy-paste clicking like I was doing before.

[AlexLachance]

I've imported a DXF from a 2D export. In hindsight this should have been obvious what was going on, but I started drawing my own construction lines within the sketch to evaluate things. Like is this feature symmetric to that feature, or is that point horizontal to that line...etc. But because the entire import was blue (unconstrained) I managed to distort some of the original sketch because it was unconstrained. So now I decided to fix the relations so they are locked down, at least as far as they relate to one another. And I think this is a bit safer state to copy/move them to other construction planes

Anyways, once 'fixed', the lines & entities turn black as expected. But inevitably there are some remnant blue dots in there. I can't physically move them. What does this mean to SW? Why wouldn't everything be black since I've selected everything within a window & its all on one layer?

The remnant blue dots are entities that are not connected to another, therefor their "end" is not defined, and the endpoint of the segment becomes blue because the segment can be stretched. If it's a line, it can be stretched "infinitly", if it's an arc, it could be stretched to do a near full circle for instance. You can select the dots and add another fix relation and they will turn black.

Maybe this image can help illustrate what I'm trying to convey