Model Not Laying Flat On Plane

[cmoher3]

Perpetual Newbie here. I have drawn an "L" shaped bracket , replicated three times and exported to Dremel Cloud for printing on a 3D printer. Unfortunately the slicer software is not putting the model flat on the bed and instead trying to print it at an angle with supports (scaffolding) under the part not flat on the bed. I'm told, by Dremel , that my Exported part, from Fusion is obviously not flat then. As much as I appreciate the transparent planes in Fusion, it leaves me feeling completely disoriented and unable to tell what is what, in terms of up/down and all points in between. Most importantly, I can't tell when my models are sitting properly on a plane. Is there a tool that will position or inform when the part is seated properly on the X plane ? Thanks.

att: Wedge2

[cmoher3]

I'm not sure how else I was to model this. I reckoned that the best way to get a matching lid was to draw a box, make it hollow and then split it. By all means, tell me a better way. Dremel does have a better slicer available, I think Cura but since I have only Open GL 1 on my computer, I am unable to install it.
I can't seem to use align as I can't figure out how to select planes, for some reason.

[davebYYPCU]

Fusion will hide construction planes, if and when used by the 1st feature involved.

There is a folder for construction / work planes, Axis and points.

use eyeballs to make them visible if and when you have a use for the same plane again.

the Origin Has eyeballs for its articles.  Hide them for clarity and I hide them when you need to use them.

Might help....

[cmoher3]

Ya, I'm just starting to find all of this out. I'll add a simpler more direct means of seating objects to my wish list for future versions of 360. The thing is, my slicer handles it with a single mouse click but when there is more than one part, it only seats one and not the other. Apparently the one part that is closest to the bed, gets set down while maintaining the other parts at their same relative distance(s). In other words, as long as I have all parts at the same distance from the drawing plane, I'm good. I can seat all parts.

I have been taking a measure of the parts relative to one another and then adjusting using move and dealing with it that way. 

[davebYYPCU]

Whilst I can't see what you are doing, 

Rule #1, should take care of that for you too,

One real world part, is a component.  

Each component built on the origin.

Use the eyeballs and activate functions, and it should be seamless.

Might help....

[Anonymous]

You said...

'and as a side note, the move command should never (almost never) be used when in parametric mode (timeline turned on).  reserve that for Direct Modeling(time line turned off).'

For all us newbies out there, can you please expand on this a little please, specifically why this is frowned upon.

That aside, I must admit one of the things I find frustrating about this software is the fact that no sooner have I learned how to use a function or feature, that I then find myself  being told that I should avoid using it.

Cheers

[chrisplyler]

The Move command (and the Align command for that matter) create situational difficulties even when used correctly, and can downright mess stuff up when used incorrectly.

For example, if you accidentally move a Body instead of a Component, you are moving that Body WITHIN its Component, meaning you are moving it away from the Sketch(s) that created it, and from its Origin.

And if you do it right, by making sure you Move the Component, then you probably should have used a Joint instead.

Stacking multiple Move/Align events into the Timeline can ultimately result in dependencies that are either unintended or misunderstood, and which easily contribute to errors when you change something without understanding those dependencies, not to mention confusion of the user. And this is all even if you use them correctly.

Trust me when I say that figuring this out the hard way, once you've put hours into a complex model, is NOT fun. You will have a MUCH better experience if you just put a little time into learning good practices in the beginning. Learn to use the Component hierarchy, model things on their origins in a logical manner, Joint things into place correctly, etc.

[cmoher3]

The thing is Chris, how does one learn these points you mention ? Have you given any consideration to making a video to illustrate the problem and solution ?

[cmoher3]

Chris, can you critique my process ?

I wanted a box with a perfectly fitting lid. I draw a box or extrude from a Sketch Rectangle. I modified it with shell. I put an offset plane nearer to top of the box. I split it and MOVED the now lid from the box, flipping it upside down and placing it beside the box in preparation for printing. So how would you have approached this ?

[chrisplyler]

Create the box and lid as two separate Components, each on its own Origin. Joint the lid onto the box, if I want them to display assembled within Fusion.

Your 3D printer software should let you arrange them. If it doesn't, you can Joint the lid upside down beside the box however you like.

[chrisplyler]

---

@cmoher3 wrote:

The thing is Chris, how does one learn these points you mention ? Have you given any consideration to making a video to illustrate the problem and solution ?

---

The Help resources available from within Fusion, various third party tutorials on youtube, this forum, etc.

I'm able to model without ever using Move or Align at all. But I do use them occasionally for convenience sake, just to temporarily get things oriented in such a way that making a Joint is easier. And them immediately after I've got the Joint made, I delete the Move/Align event. Same thing goes for dragging an item and then Capturing Position.

A lot of trouble can be avoided by correctly modeling things in the right place to start with, when it's practical to do so.

[Anonymous]

Is the Move command also to be avoided when using it to make copies?

[chrisplyler]

I avoid it all the time. If you're working smart, you'll find you don't need it, except for the occasional "move something just to see or be able to place a joint conveniently, then delete afterwards" described above.

[laughingcreek]

@cmoher3 -

attached is how I approach box type designs.  I also made a screen cast of me fiddling with it (changeing the size, etc).  I suggest stepping through the timeline and editing each feature to see how things where done.  Note all sketches can go on origin planes for this type of design, which helps simplify things.  At the end of the screen cast I used a joint to place the lid on the same plane as the bottom of the box.

Looking at your designs, I can see your design mind set is what I refer to as a "cut and past" mind set, which works well for things like photo shop and tinker cad.  But this approach doesn't utilize the way a parametric modeler like fusion works, and will just cause you headaches.

my suggestions for moving forward-

-forget about using the primitive shapes like box and cylinder.

-forget about using the move command

-go through the tutorials on sketching and get really good at it.

-start exploring the solid modeling features (extrude etc...)

-learn about components, and then do a forum search for rule #1 (and then go back and learn about components some more.

-wash, rinse, repeat

https://knowledge.autodesk.com/community/screencast/1567e8c8-c1a6-45d5-af6d-50949cd1cebd

[cmoher3]

Very cool approach !!! I'd love to see this as a video.

As a newbie, you know I have questions:

That vertical meter/yard stick running up the side with all the bubbles on it, I don't know what it is or where it comes from ? That and some other items I did not see on the timeline.

I also noticed solid black dots in those corner braces. I don't know what they are. Did I miss them in the timeline ? I also noticed the appearance of a couple of boxes in the timeline, but you had said to avoid their use. Did you mean 'use them but sparingly' ? 

I was really intrigued by your ability to extrude graduated shells. When I went to select those faces, for extrusion, I was unable to do so. I got either lines or entire bodies. Did you just use the Selection filters to do that ? 

For example, you drew out those shell lines in sketch mode, changed the selection filter to faces, and selected all of the faces for the first short extrude....... would that be correct ? This is one of my biggest challenges, is just getting certain features selected for work without getting just lines or much bigger, inclusive selections I don't want. I noticed my magnification can sometimes play a part and the selection filters I'm having a hard time getting a handle on. Could it be that my computer's graphics capabilities are too weak ?

This is a very interesting approach and I'm very grateful for your time. What a cool, and no doubt better, way to do my projects.

[cmoher3]

Went back in for deeper looks....so Sketch one was locked down and then you started on Sketch 2 which appears to be Construction markers for extrusion heights ? I do not see this sort of construction under that menu but it is a great approach. It appears to me at least to be a construction of a 3D lattice, followed by a series of extrusions.

[davebYYPCU]

The ladder or yard stick, is Sketch 2.  For construction purposes, but not to be found in the construction menu.  

You have to make it, it marks out the height of all the features.  Extrude To Object, - selecting the end point of the marker,  means Fusion will transfer that value.

Change the sketch dimension, the Extrude will update.

The black Points are either mid Points or radius points or both for the hole/s.  Black because they can only move with change of dimension it has associated to it.

Setting up like this makes for saving out various boxes from a master design.

If you don’t need to go that deep, Extrude to a value and you can later change the value, 

6 of one and half dozen of the these means you can get the same thing various ways, comes down to how you know how to do it.  

 Might help....

[chrisplyler]

Okay, I opened up your file of the box and lid. I would like to explain that Fusion 360 is not SketchUp. But you are using it like SketchUp. Instead, Fusion is a PARAMETRIC modeler. Big difference. If you want to use it like SketchUp, okay, but you're sacrificing the huge benefits that come along with parametric modeling.

I made a Screencast video for you. It's kinda long. I start from scratch and walk you through the box and lid that you've made. You aren't suddenly going to be an expert just from watching it, but hopefully it will open your eyes a little bit.

Screencast video:
https://knowledge.autodesk.com/community/screencast/2ad9c330-753e-4e00-b707-ed1d8663ad0b