Joining line segments (x,y coordinates) in a sketch into one line.

[lmorgan5L3UA]

I have inserted csv (X,Y points) which imports well over 150 line segments.  How do I join the line segments into one line?  This becomes a big problem down stream in CAM as it is near impossible to get all the segments to run a contour for mill cutting a rib.   Sample attached.  I have not been able to find a method to join the segments.  

Old school Autocad 2000 had Pedit to be able to join and create a contineous line segment.  

I am a newb with Fusion 360, it has been a challenge but I have enjoyed some of the features.

                     ..Lynn..

[Leo_Dyn]

If they are all co-linear, consider just drawing a new line from the first starting point to the final endpoint? As long as you make sure those two points are coincident you should be good to go.

By the way, if you are not using all those line segments for anything else, you could also consider selecting them all, and hitting the 'x' button to make them construction lines.

[Bunga777]

If I close this sketch like this and then extrude it with Extrude, I can follow its contours with CAM, but is that not enough?

[jhackney1972]

I have converted your sketch into one segment.  Video will prove this.  Model is attached.  If you need any help understanding my method please ask.

[jhackney1972 · Accepted solution]

If you do not want to create the smooth sketch, as I showed in my previous post, you can use your existing multi-segment sketch very easily to create a CAM toolpath.  The video will show how.  Model is attached.

Do not forget to "Accept Solution" if this solves your question, if not, please ask.

[lmorgan5L3UA]

Hello John,

Exactly what I was looking for... Many Thanks!

..Lynn..

[lmorgan5L3UA]

Hello John,

The method looks good, is there a way to get an outside cut, currently it is cutting the inside of the profile.   I had a later version of the rib with more details added, and a bunch of experiments on it is a mess by now.  I need to redo to get things straight.  

Additional detail: I need to add couple of breaks in the profile to hold the ribs in place while cutting, I typically cut two sheets stacked at one time.  

                           Thanks...   ..Lynn..

[jhackney1972]

The toolpath I attached is cutting outside.  You will need to supply a bit more information as well as some screen captures of what you need and of course the model.  

[jhackney1972]

If you mean to run the toolpath on the opposite side, which is inside to me, here it is.  You will have to have a lot smaller tool to reach the end.

[lmorgan5L3UA]

When I first used your technique, it worked but the end mill cut on the inside of the rib pattern, I need it to cut on the outside of the rib pattern.  In reviewing your video, yours did cut on the outside of the rib pattern which is what I need.  How did you change the side that the tool cut on?

You were able to demostarte it can be done, but I'm not sure how to do it.  

Sorry my milling terms are lacking, my hobby is radio control airplanes and am cutting balsa, 1.5mm end mill, for a modified wing I am in process of building.  

            Thanks for the help!          ..Lynn..

[jhackney1972]

It is a simple setting under the Geometry Tab.  Video and screen capture should show all you need.

[lmorgan5L3UA]

Ah....Yes, that is very nice button to have!  Unfortunately I am using the non-commercial (hobbyist) version and my Geometery menu does not have that button.   Hopefully the screen dump made it to the attached png file.  

When I have used manual selection on desired contours, I get a red arrow for indication on which side it will cut, toggle the red arrow and I get the other side.  

Guess I might go back to old school Autocad 2d and CAM software.  It seems a bit sad that this type of functionality isn't integrated into the non-comercail version.  I really appreciate all your help and very quick responses!   Looks like I need to close this out as it appears to be a dead end street for me....

                     Happy Holidays!         ..Lynn..

[jhackney1972]

I have access to a Fusion 360 Personal License as well.  You can achieve your desired result if you first convert your segmented line into single continuous line, as I showed in message #4 of this Forum question, and then you will get the inside/outside selection.  The video will explain.  If you need help with the process of converting your multiple segment line into a one continuous line, let me know.  Model is attached.

[lmorgan5L3UA]

Hello John,

Contineous line solution looks promising.  What is the technique used to convert segmented to contineous.  Hopefully I can add breaks to the contineous to add detail.  

                     Thanks...   ..Lynn..

[jhackney1972 · Accepted solution]

The process I used takes a little time but is not hard.  The spline created by the process is a continuous line and can be selected "directly" from the graphic screen in the Manufacturing Environment.  When you do this you can select the arrow to go from inside to outside toolpath as needed.  The spline created is just a sketch, you can add or subtract from it as needed.

[lmorgan5L3UA]

Hello John,

Agree with the convoluted approach but it appears to work!  Most of my Cad work can be done in the 2d world so I do not have any Mesh experience, something to do in the future!  Maybe I'll get a chance to try the process out this afternoon.  

I am still amazed the Fusion does not have a simple 2d tool to do this job.  It appears this has been a request for many years, it's been in the AutoCAD product for well over 20 years and is a time saver.  I will need to evaluate the process as I have 32 ribs that this has to be applied to.  At first guess, I'm thinking the 2d AutoCAD and Cam is going to be much faster to complete the Cad-Cam work.  

                  Very Much Appreciate your expertise and quick help!    Happy Holidays        ..Lynn..

[david_desboisHMJ74]

This is Exactly what I'm trying to do!   I unfortunately am not successfully reverse engineering your steps in your provided .f3d file to get to the end state.  Would you be able to write down a few of the steps to get from the csv file to the Mesh Section1?

UPDATE:  I think I got the steps figured out:

1. Create the sketch from the CSV file. Finish sketch.

2. Click the Sketch and Extrude it a bit.  This creates Body 1.  Note: we only need to extrude a few mm because we will make it a mesh next.  Then we will use the mesh outline to make the solid line with a spline.

3. Click the Mesh tab.  Click Create --> Tessellate.   Select Body 1.  Note: I just left the defaults and click Ok.  This turns Body1 into a Mesh Body1.

4. Click the Mesh tab.  Click Create -->Create Mesh Section Sketch.  Click Body1 (the new Mesh body).  Rotate the Section Plane to be the outline from the CSV file (in this case it's the airfoil shape.)  Click OK.  This creates Sketch3.  Sketch 3 now has an orange colored line.

5.   Right click Sketch3 --> click Edit Sketch.  Click Sketch --> Create --> Fit Curves To Mesh Section.  The "Fit Curves to Mesh Section" dialog box opens.

6. Edit Fit Curves to Mesh Section attributes.   Select either Closed Spline (if the line is continuous) , or Spline if it's just a line.  Click OK.  the Orange line changes to a Blue line.   Finish Sketch. 

7. Extrude the Blue line.  Click Solid --> Create --> Extrude.   Ok

8. Bonus- if you are trying to fillet the airfoil connection to another body, use a box and cut the tail a bit to make it square, then it will fillet nicely. 

If you see anything I missed let me know.   Thank you!

[TheCADWhisperer]

@david_desboisHMJ74 

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