Is this type of plane possible?

Hi,

I am trying to work on a shelf I am building, and I am fairly new to Inventor and have watched a few hours worth of tutorials. I use 3ds max heavily and was able to make this angle with no problem. Take a look at the images and see if maybe this can't be done in inventor.

I tried a 3d sketch, but cant get that to extrude. thanks for any insight!

[ATTACH=CONFIG]46810[/ATTACH]

(a) your attachment is invalid, so I can't look at it.

(b) You can only extrude a planar - i.e, 2D - sketch.

see if this works.

Okay. See, what you're showing there is not actually a plane. It's 2 quads, which are themselves non-planar. Yes, you can create a boundary patch to cover each of them, if you want.

BUT ... it's important to really divorce yourself from the 3DSMax mindset. Inventor works completely differently. It's a lot more like actually manufacturing the part, in a lot of ways.

Scribble up a napkin sketch of what exactly it is that you're trying to build, so we can see what your design intent is. We'll take a look, see if we can't figure out how to help you make it.

Okay, based on your picture from Max - which seems to have disappeared? - it looks like this is more or less what you're trying to do?

shelf plane.ipt

that is the same result i got also.That middle 4" channel should go all the way down the center. and the sloping should start at that edge, and slop down towards the center. Its hard to explain.

Do you want your faces to be planar, or do you want them to be organic? Either one is possible.

shelf plane.ipt

Try this ...

Oh that is perfect, thanks! I love how the parent/child system works compared to max. You can really learn a lot from different methods by examining it.

Glad I could help! Good luck with learning ... keep coming back to ask questions, we'll help you figure it out.

So from the looks of it, I should be building in a quad format if making furniture pieces like this, and then mirroring them since they are symmetrical.

Something like this, where it's symmetrical, it was just easier to do it that way. No sense doing the same operation over and over again when you can let the machine do it for you. This is one reason why it's good to build with a definite relationship to the origin planes in mind.

One thing to note, though: when I did the mirrors, I mirrored the whole solid, not the feature. Split features cannot be patterned.

What type of constraints did you use on "Sketch3"? When i try to rebuild this from scratch, and i increase the distance of the centerpoints like you added, it expands the entire size of the sketch, rather than move the point up and down the edge.

On sketch 3, I projected the edges at the short ends as construction geometry. I dropped a pair of center points on them, which automagically creates co-linear constraints, so long as I get the points on the edges. I dimensioned one of them 2" away from the end of the construction line, and used a horizontal constraint to bring the other point in line with the first one.

It sounds, from what you're describing, like you're not using projected edges to hold things in place. When your geometry is not otherwise constrained, the first dimension that you place and set will re-size everything in scale with however you changed that first dimension.

(On sketch 2, I just dropped the point onto the mid-point of the projected edge.)

how did you get that Extend1 function underneath the boundary patch. I have the boundary patch and when i trim it gives an error. So i assume that Extend1 has something to do with it.

You want to use split, not trim - trim is for cutting back surfaces, split is for cutting geometry.

But, yeah - extend takes the edges of the surface away from the solid, so that there's no ambiguity as to what exactly you're cutting. It's in the pulldown below the surface tools on the 3D model tab. The .875 value isn't magical or anything - it's just the last value I used for something else, so it popped up as the default here.

Also, with the split tool, there's a few different things you can do, and the default is to split faces on the solid, not to cut away material.

(BTW - how do you like the boolean operations in Inventor? I came up using Lightwave, and I really, really love not having to worry about n-gons and all that stuff, or whether or not my boolean was going to fail, or how it would affect the poly flow, etc. I haven't fired up Lightwave or Modo in YEARS now. Switched to Inventor and haven't looked back!)

Sorry, i meant to say split, not trim. Now I got it. This is going to take some habitual use to really get this down. from the small bit i have used for boolean in inventor, I love it. 3ds max has a pro boolean feature which is pretty nice. But I just like the fact of building objects using real world dimensions then pushing them to max for final tweak and render.

How can i get these squiggles to be straight? After I Split, it creates these in the image.

How can i get these squiggles to be straight? After I Split, it creates these in the image.

 

[ATTACH=CONFIG]46818[/ATTACH]

Attach your model, let's have a look. It may be something simple.

If it's Inventor 2013 or earlier, I can take a look here while I'm at work. If it's 2014, it'll be tonight before I can do it - I only have 2014 at home.

It's 2014, so no worries. Although, when i place a shelf side on the drawing, the Extend / Patch is showing. How can i hide that?

http://www.starkform.com/plane.jpg

I solved my problem. I also started using the loft function to create these shelf profiles which is working out nicely.