Sketch offset, curve selection?

[and.ranch]

Hi there,

I simply can't figure out how to make this works:

I've been trying a couple of times to do offsets of loops in sketches, but unless i use e.g. the rectangle or circle tool, i can't get the offset tool to recognise a sketched loop. It either doesen't include a line in the loop, or gives me the error "cannot offset beyond this point", which i interpret as if it is trying to offset beyond the sketch itself. 

I've then tryied to go around and select the lines to do the offset from, but i then hit the wall because the tool doesen't allow for selecting multiple lines, which makes it practically worthless.

Hope i'm just missing something, and you can help me out!

[FrankCao]

Hi ovisopa,

Thanks for posting the question. 

I had a look at your file and I think I understand your problem. In your sketch imported from DXF file, some curves are only visually connected in position, which means, two lines could have 2 endpoints located at same position, but there are no coincident constraints connecting them together. In this case, we don't think the lines are part of a "curve chain". You can try a simple case in Fusion sketch as draw two connected lines, then hover on the middle connection point, select the coincident constraint, then delete it. In this case, you end up with two lines visually connected, but they are not really connected. (There are two endpoints at the same location.) When computing sketch offset, Fusion only recognizes "real" connected curves as chain, and then you can select them all with "Chain Selection" enabled in offset command. To fix your problem, you could try add coincident constraint between the two lines to make them really connected. To know whether the lines are only visually connected or really connected, you can try left click on the connection point without releasing the mouse button, then the context menu would pop up to show you the detailed point information like follows:

Then the problem could be why after inserting dxf file, Fusion doesn't help create coincident constraints automatically between two points at same position? The answer is Fusion wouldn't add constraints automatically during the dxf insert workflow. Two lines either would share same endpoint during insert(in this case, they are really connected), or would have two points located at same position based on how dxf file stored the detailed points information.   

But when computing sketch profile, Fusion uses a different algorithm that as long as the lines are overlapped/connected in position, they can form a closed profile. A simple example could be, you can draw two overlapped sketch rectangles without adding any constraints between them. Fusion will intelligently compute the profile of both rectangles and the intersection/union of the regions as sketch profile.

Please let me know if you have more questions.

Thanks,

Frank

[ovisopa]

Thank you @FrankCao I talked to the client and asked him if there is anything he can do regarding this problem I have with the DXF files received from him, they made some adjustments, they told me the first thing he did was to make sure all the lines and arcs are pointing in the same direction, than just before export, he joined all the lines toghether. After those steps I could import his DXF file and Fusion recognized the contour as a single contour, when I tried to apply the offset, it went just fine, as it should, the entire contour at once. But before he sent me the modifyied dxf, I tried a few suggestions.

My first problem was placing the coincidend constraint to all the line, did I understood correctly the each line end point needs to be coincidend with the next line start point ? It was difficult for me to chose the points as the end point of a line was in the same position with the start point of the next line, and when I tried to click the coincidend icon, than click on one line start point, when clicking next in the same point where the other line end pint was, nothing happent.

How I should add the constraint on two lines that have ones start point and other ends point in the same visual location ?

Appreciate your effort.

Wish you all a awesome weekend.

[FrankCao]

Hi ovisopa,

Thanks for the question. Yes, it's a bit difficult to add coincident constraint here. And actually fusion asks you to add coincident constraint between one endpoint and a curve.

So in your case, if you know where the curves are only visually connected, you can try drag one of the curves a bit to make those two curves separate. Then you can try add coincident constraint between one curve's endpoint and another curve. After that, you should be able to extend the offset chain.

Thanks,
Frank

[CruftMeister]

Ovisopa,

Thanks for reviving this thread, I too am struggling with the limitations (this is my perception at least) of the offset command.  I've projected edges from some 3D surfaced geometry and need to offset the projected lines, but am not able to select more than a few of the edges at any one time.  I don't know if the Fusion team considers this a "bug" but perhaps it is a candidate for the "Support" forum list . . .

[5X-machines]

Hi everyone,

I decided to resurrect this thread as its 2019 and I am still running into the  exact same issues all of you have described. I hope the devs recognize this and will improve offset curve soon. It seems like a rather basic feature that has worked flawlessly in every other cad I've used.

[TrippyLighting]

Post a file, describe the problem and we might look into it.