Using Offset on Sketch drawn with Spline tool

[Anonymous]

I have drawn a sketch consisting of a couple of lines and some splines creating a closed loop. I am having trouble using the offset tool. I would like an offset of 24mm inwards. My sketch is not fully constrained. I sustpect hat could be the trouble. Not sure how to fully constrain splines. I hope someone would take a look and help me out. Thanks!

/Mark

[James.Youmatz]

Hi @Anonymous,

Were you having trouble creating an offset in general, or having trouble selecting the whole perimeter at once for your offset? I was able to create the offset for your sketch, but I had to use the offset command twice as it didn't loop fully. I went ahead and created a screencast showing how I created the offset.

http://autode.sk/1Jrtbzf

Hopefully this clears up the issue you were having and if so please feel free to mark this answer as a solution so others can benefit from this thread as well. If not, please let me know and I would be more than happy to keep helping!

Thanks,

[Anonymous]

Thank you James for the screencast. I am able to perform an offset as you demonstrate in two parts. What I need is to select the entire loop and offset in one go. This should allow the splines to scale correctly. What you are showing causes a problem as seen on the attached screen grab. I have zoomed to the top left corner to show how the offset is performed correctly here, but incorrectly in the top right corner where the "two part offset" becomes joined. The top right corner looses it's shape to the original.

Is there a way I can work around this?

Thanks

/Mark

[kellings]

What is your desired end result? Another method you could use (which I probably would do) is to draw your first shape and extrude that shape.

Start a new sketch on that face and then use the project geometry command and click on the center of mass of the face. That will project the outside loop of the sketch in one click. Iw as then able to offset that projected geometry as one whole loop. 

Let me know if you need me to do a Screencast. I was going to but it isn't launching correctly right now. I probably need to restart or something. 

[Anonymous]

Project Sketch is a new one to me 🙂 I have done as you suggest and it achieves the same result as before - the top right corner is not rounded correctly.

What I want to acheive is a scaled down version. I have tried scale which works great, but then when I go to edit the scaled sketch it jumps back up to the size it was before the scaling factor? Now that I am aware of the Project Sketch funtion I have come up withe the following work flow that achieves what I want:

Edit original Sketch.

Select all, right click, Copy.

Close Sketch.

Create new sketch.

Paste.

Close Sketch.

Create new sketch.

Project intermidiate scaled sketch.
Close Sketch.

Delete intermidiate scaled sketch.

I now have the original sketch intact and I have a scaled version that I can work with. Now when I edit the new sketch is remains at the scaled size because it is no longer a scaled sketch but a projected version of the scaled sketch that is now deleted. I'm sorry if I confused you with all of this.

If you have a better solution let me know, if no better solution also let me know and I will simply set this thread to "Solved".

Edit: This poses a new problem. I can't seem to move, edit or select this new projected sketch?

Thanks

Mark

[James.Youmatz · Accepted solution]

Hi @Anonymous,

Sorry it took so long for me to get back to you. I looked into this and I think I have an answer to most of your questions.

1.) To address your edit about moving the projected sketch: when you create a projected sketch it creates a link referencing it to that original line. You will then need to go in and break the link in order to move it. You can do this by editing the sketch that the projection is in, then right-clicking the projected line and select "Break Link". This can be seen from the following screencast at roughly the 10-20 second mark.

http://autode.sk/1Jty3tP

2.) By deleting your construction lines, I was then able to select your spline in one-click as a whole. NOTE: This will still create the abrupt point in the top-right corner of your offset. This just has to do with the way your geometry is. You can only offset that smaller so much before that rounded edge starts converging to a point. A few suggestions I would have is to either scale the spline up (so recreate the spline smaller and then offset it bigger by 24mm). Another suggestion (and perhaps more complex method) is to view the curvature comb of the curve you have created. You will want the comb to look as gradual as possible indicating a smooth curve. This may make a smaller offset possible. You can smooth the curve out by doing a few things. The first is to delete the tangent constraints that are around the curve in the top-right corner of your spline and replace them with a smooth constraint from the sketch palette. Also you can move around the tangent lines (which I show in the screencast below) in order to try and create a smoother curvature comb.

I know #2 was a lot to take in so I created a screencast below detailing how I went about those steps. I ended up learning a lot about sketches so I thank you for coming to us with this problem! It's a learning experience for us all!

http://autode.sk/1PUlIxZ

 This screencast should show you how to perform all of the steps I outlined above in #2. Please note that when I was selecting my tangent handles (they were originally green and then when i clicked them they became blue and i could move them and manipulate them) I was just trying to show you that is how you do it. Please don't think that what I showed was a good final example of what your curve should look like! I was going fast to keep the screencast as short as possible 🙂

I know that was a lot of information to take in, but please feel free to ask me any more questions you have and I will try to answer them to the best of my ability. If this answered your question, please feel free to mark this answer as a solution so others can benefit from this thread as well. Also the link I'm posting below is a really good forum discussion about curvature that you may want to check out!

http://forums.autodesk.com/t5/design-and-documentation/when-using-smooth-constraint-why-are-curvature-handles-hidden/td-p/5498274/page/2

Thanks,

[Anonymous]

Thanks James,
This gives me some options to work with. At the moment I prefer for this project to copy a protrusion, then scale that and project to a new sketch. That's nice and clean and get's me where I want. Great support - thank you!

Mark