Extrude to construction line on 2nd sketch

[SGoldthwaite]

I  have a pretty simple object - It's a plate with a sketch on the bottom that defines the outline of the plate, and an inner area.  And another sketch on side of the plate with a construciton line.  I extruded the outer perimiter 3/8" just fine.  Now I want to extrude the inner section a bit less than that.  I want to extrude it to the construction line on my side sketch.  But when I use the Extrude To tool, I can't select the construction line as the "to" point.

I thought maybe using the Include 3D Geometry function might help.  So I went to edit my bottom sketch and intended on adding the construction line from the side sketch as 3D geometry.  But when I went to edit my bottom sketch, my side sketch was not visible, not even in the browser.  So I was unable to give this a try.

Here's my model: http://a360.co/1DzNZpC

Also, is it possible to extrude the inner section to a fixed distance from the outer extrusion?  Let's say I wanted to extrude it 0.06" less then the outer extrusion, regardless of what the outer extrusion is.

[martin.zatecka]

Hello,

your side sketch isn't visible because it is newer part of your design. When edit features you can see only the existing features. Don't worry, it isn't necessary at he moment 😉

Let's look at the extrude, please follow next steps.

- open extrude

- select the sketch

- open "distance" and select Measure

- measure height of extrusion at any corner, the sketch isn't necessary.

- measured value is automatically set, so just add your correction (- 0.06) and press ok.

regards

Martin

[Anonymous]

Just for future reference, you can also try moving things in the timeline further back, to change the order of things.  But if say a sketch depends on an earlier sketch, Fusion will not allow you to move the latter before the former.  Just something to keep in mind.

Jesse

[SGoldthwaite]

I should probably clarify what I was hoping to accomplish.  I wanted to extrude to the construction line so that if I ever changed the position of the construction line, the extrude would change wiht it.  Similar scenario for my question about extruding to an offset distance to the first extrude.  If the second extrude was 0.06" less then the first, then I changed the first, the second would change with it.  Basically I wanted to link them.  I really like how you can link things in the sketches, so I'm really just trying to learn where else, if anywhere, I can do that.

[Anonymous · Accepted solution]

One option you have is to use/reference parameter names.  In this video I do this for using simple parameter equations to define offset planes, which sketches are defined on, and ultimately in the vid example which a loft and a cylinder are defined by.  But the same method would apply to just simple extrude distances.  The first 4 minutes, especially after minute 3, is relevant to showing this:

https://www.youtube.com/watch?t=200&v=HvOV38d8JIo

You can also access these parameters in the 'Modify parameters' under the Modify tab.  Using parameters is really powerful because it works across sketches, 3d operations, and time, with no limitations 😉 Let me know if you have any questions.

Jesse

[martin.zatecka · Accepted solution]

Hello,

I prepared an example of your design. You can link parameters similar as in Excel.

For input you can use user parameters, but it isn't necessary. You can link parameters to Expression column, or even write an expression to "distance" when extruding. Parameters table allow you any future edit and shows relation between parameters. For example change an expression of height of inner extrude to WB_t - 0.06. It is open for various solution.

regards

Martin

[SGoldthwaite]

Thanks Jesse, good video.  I watched the whole video, and your essentials video also.  Now my head is spinning, this stuff can get pretty complicated!  

Linking the 2nd extrusion distance to a parameter in the sketch is exactly what I wanted to do.  

[Anonymous]

Hi Scott, really glad you found the vids useful :).  Don't let the video with that weird time traveling workflow throw you though, I don't normally use that workflow, and also I do in fact try to always activate components to get sketches and everything to go into proper components, I just didn't in the vid for sake of demonstrating what a nonpunishing workflow would look like (i.e. no consequence of forgetting to do something at some point).  Just for sake of completeness I'll mention there was a thread discussing this time traveling workflow, and potential future timeline behavior, but like I said i don't normally use any of this: http://forums.autodesk.com/t5/general-fusion-360-questions/my-workflow-and-future/td-p/5559908/highl...

Good luck, it can be really fun to learn Fusion360!

Jesse

[Anonymous]

I should also mention here regarding the joints video, that I try to use them sparingly, electing instead to try to build stuff in place, and always defining new stuff on the faces/sketches/work planes of existing "old" stuff, so everything parametrically updates well.

Jesse

[Anonymous]

Hi Scott, since you seem really up to learning Fusion360, I put up this tip of a great collection of short screencasts for learning. 

http://forums.autodesk.com/t5/post-your-tips-and-tutorials/collection-of-short-screencasts-for-learn...

Jesse

[SGoldthwaite]

Yes, I'm really trying to learn all I can.  I've been watching all the youtube videos and did one live classroom and signed up the the one next Tuesday.  I looked to see if there was a formal class I could take, but I didn't find anything.  It looks like there is a lot to learn.  I've come over from the SketchUp universe.  Fusion 360 is really impressive and I really like how they've integrated the CAM.  I'm really trying to get into the digital manufacturing (for fun, not a career).  I have a laser cutter, 3D printer and Shapeoko CNC router.  I'd really like to get my hands on a CNC milling machine like a Tormach. There are a couple small maker spaces in NJ, but they don't have the CNC mills or lathes. 

[Anonymous]

Impressive your tenacity.  Yeah, it's a very exciting time we're entering, for the whole world ;).  Fusion 360, coupled with continued hardware revolution, is really what is going to change the world for the better, hopefully beyond what we can even imagine, in the near future.  It's all about empowerment of the person. 

I will soon be releasing a dirt cheap machine that competes with the Tormach in rigidity and capability to machine metals, but using very new machine design methodology.  Stay tuned!

Jesse

[Scoox]

So, just to clarify, Extrude To Object only works on 3D features, not sketch geometry lines, correct?