extend tool in sketch

[Anonymous]

Hi, I am a beginner following one of the webinars, and for some reason when I use extend tool under sketch, it does want to extend from the same end point of the line as shown in the webinar but will extend from the other endpoint of the line as shown in the attachment. How can resolve this?

thanks

[FrankCao]

Hi ramadanramsey,

By looking at your post, do you mean the line is extended to some strange place where there are no real intersections? 

Currently Fusion 360 will extend a line to any closest line "without boundary", which means the line will be extended to another line's virtual extension part. Please look at following picture:

Actually the line will be extended to the first line although the first line has no real intersection with the line to be extended. Fusion will treat any boundary line as endless length. 

So if you want to extend the line to the second line in the above picture, you can try extend twice.

Hope above suggestion helps!

Thanks,

Frank

[Anonymous]

thanks Frank, referencing your picture, imagine there was another vertical line on the right side of the screen, my extend tool works fine when making an extension to the left line as shown in your picture, but I cannot get the extend tool to extend the line to the right side of the picture where I have another vertical line. that is my ongoing dilemma: choosing the side my line extends from,

thanks

[Anonymous]

I d also like to add that i used the offset tool, so the two vertical lines are the same distance from the horizontal line I wish to extend

[jeff_strater]

I may be missing something, if so please let me know.  But, the sketch extend tool is sensitive to which end of the line you hover over.  If you move the mouse nearer to one end, it should extend that end, if you move towards the other end, it should extend that end.  I have tried to re-create your example in this video:

If you are seeing behavior that Extend does not work this way for you, there may be a bug.  If so, if you could share your design, it would help us get to the bottom of it.

thanks,

Jeff

[Anonymous]

Hi, attached is the file design. Like you said, it should extend from both ends but mine does not, thanks again for the help.

[jeff_strater]

Hi @Anonymous, I apologize for the delay.  Thank you for sharing the file.  I can verify what you are seeing.  This is strange.  It seems to be only that one edge that has the problem.  I will report it to the sketch team to look at.  

Jeff

[jeff_strater]

Actually, the problem is worse than I thought.  Basically, Trim and Extend do not "see" the edges of the face.  This is wrong.  We'll fix that bug.  Thank you for reporting it.

Jeff

[pete]

I am not sure if this is relevant here but I often fight with the extend tool in  Fusion360.  It will often only extend a very short distance when I am trying to extend to another line. Many times I will have to click extend several times to go a very short distance.  This is quite frustrating and time consuming.  I do not see any reason for this behavior based on the software settings. Trim seems to work as expected but extend often will not only fight extending to an adjacent line but it will also seem to take several seconds for the command to respond.  This seems to be the only command that behaves like this.  I am not sure if I am doing something wrong or if there is a bug or something but it would seem an extension command should extend to the next available geometry and stop not extend to some random short distance from the start point.  Am I missing something here?  Thank  you..

Pete

[TheCADWhisperer]

---

@pete wrote:

... not extend to some random short distance from the start point.  Am I missing something here? 

---

My guess is rather than random short distance - it is actually extending to a projected intersection with other geometry.

Is there a reason that you can't simply click and drag the white endpoint?

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[jeff_strater]

@pete - @TheCADWhisperer is correct here. The Extend behavior is not "random", Fusion uses virtual intersections in Extend.  See this screencast for a simple example that illustrates.  This is something that we debated before the initial implementation, but the added value of being able to have virtual intersections outweighed the costs.  Think of this case: 

without virtual intersection support, you would not be able to use Extend to close this profile.  You would have to first drag one line to intersect the extension of the other, then Extend the second line, then Trim off the excess.  With virtual intersections, this is just two Extends.

[pete]

This is what I figured would be the expected behavior of the tool. However even on a single initial sketch I find that the extend tool will make a very short extension repeatedly to no particular adjacent line or geometry.  I mean it will give very short perhaps say there are two lines 1 inch apart and you are extending one line to the side of the other line. The tool will make like ten or more very tiny extensions and each time seems to have to think about it for several seconds before the tool is completed with its job.  I have seen this on complex and simple sketches, I will admit that some of my sketches are often quite complex but again I see this behavior even in the initial stages of the sketch.  If it worked as in your screencast I would be very pleased because one can obviously see the benefits of such a behavior allowing it to stop at the extension point of adjacent geometries.  This is not exhibiting this trait.  So back to the 1 inch apart geometries, it will give you a tiny extension perhaps 1/32" long repeatedly until you can get it to the point you are trying to extend to. 

   You asked about grabbing the end point and extending it. I often do this as well. However I find that SOMETIMES if I am not careful with how I drag it the snap behavior of the line can not only cause undesirable locations snaps but  can even upset other geometry that has constraints already in position.   We are using Fusion360 all day every day in a commercial environment so this can become cumbersome.  

   Perhaps it is my autocad background but I often draw complex geometries using offsets and construction lines and then remove what I do not want so I use the trim and extend features a great deal.  To be honest I am quite pleased with Fusion360 aside from a few annoying things like this.  

[pete]

Another odd behavior I have seen lately is that the extend tool will, when it appears to function properly, extend the line to the adjacent line.  Then when I go to close the sketch I find that the extended line JUST BARELY does not make it to the adjacent line when I zoom in. I have to then extend again to close the shape. Again this does not appear to have any relation to any adjacent geometry.  We are a custom cabinet and millwork shop making wood and metal projects and most parts are set on appropriate geometric tolerances that would have no need for adjacent geometry that tiny bit away from the extend to line.  I hope my descriptions here are making some sense.  To be sure when the extend tool works  as expected it is a very welcome tool and I use it very often.  Just have been seeing this strange behavior a lot lately. It seems to really slow down the computer when it is " thinking" as well which only exacerbates the problem.  I don't pretend to know what is happening under the hood during this momentary pause but presumably it is comparing sketch geometry to extruded solid parts and making the resultant adjustments but I would think that would happen all at once when you close the sketch no?  

[jeff_strater]

if you can show an example where it is behaving in a way that you feel is wrong, we'd definitely like to see that.  I'm moderately familiar with the workings of this, and it really should only be extending to virtual intersections.  Remember that a virtual intersection can be to a closed line as well:

and that the virtual intersections are not limited by proximity (they could be way on the other side of the sketch), and finally, if you sketched on a face, and have auto-project on, each edge of that face is also in your sketch, and can result in virtual intersections.

[pete]

https://autode.sk/3l2bSzh

Tried to make a quick screenshot video of the problem. I am not sure if it is clear what is happening here but it does show the extend line snapping to a spot that seemingly does not line up with anything else vertically in the sketch or horizontally for that matter. This instance it actually went farther to the stopping point than it normally does. Most times it would take several extension commands to got his far.  It also stopped each time on different distances from the start point even though the lines are being extended from the same point vertically.  I do indeed often project geometry from a face but I do not use that feature global setting to project every sketch I use the project feature when I need to create geometry relative to another part in the model so only when I select it.  This is a built in cabinet setup we are working on and it only has really vertical alignments and as you can see from the sketch there do not seem to be any geometries in that area to extend to... 

Pete

[jeff_strater]

can you share that design here?  Remember, it's not just horizontal and vertical alignments - any line anywhere in that sketch at any angle can be a virtual extension.  For example, here are some lines that would be easy to forget about:

even the shortest line segment anywhere in the sketch can be a target.  Like some of these:

so, imagine that you take every single line in your sketch and draw those lines as far as possible in both directions, that is the set of lines we are extending against.  In a large sketch like this one, that can result in quite a rat's nest of lines (and is also why you get those pauses in Extend - it is looking at every one of those lines).

I don't think we do virtual intersections to arcs/splines (though I'm not certain why not, to be honest).

[etfrench]

In sketches where there are lots of virtual intersections, using the collinear constraint can save a lot of time and key strokes/mouse clicks.

The Trim and Extend tools could easily be fixed by adding a 'To' field and let the user select the geometry to extend or trim to.

[pete]

Yes indeed a "to" feature would simplify this a great deal and work much as it does in Autocad and other programs.  I have experienced this same behavior in simple and complex drawings.  I just pulled angled lines from the corners of all the doors on the base cabinets and none of them seem to align exactly with where the extend lines stop.  I  may be missing something but I checked every one. Most are not even close to this point and the fact that they extend to different positions within less than 1/32" of each other makes it even more unlikely that they are extended to some random geometry elsewhere in the drawing.  

[jeff_strater]

@pete - if you could share the version of the design where you removed the angled lines (or any version, I can remove them myself if you've already discarded that version), I'd be happy to take a look at it, and see if I can figure it out.  Thanks.