2D sketches on 3D plane?

[Anonymous]

I’m trying to learn fusion for cutting sheet metal on a plasma table and I need help with learning how to design/sketch 2d sketches in a 3d space for ease of the design process. I’m trying to draw individual sheet metal pieces that with assemble with a tab and slot system and be welded together producing a 3d finished product. Each individual piece with remain a flat piece of sheet metal so as far as I can tell it is not the sheet metal workspace that I need be concerned with. Right now I’m doing these sketches in an orthographic manner but I feel like there has to be a more efficient way to do it. 

Im not sure what terminology to look for to learn how to do this so I just keep finding irrelevant information. If anyone can point me in the right direction I would greatly appreciate it. 

Attached is a rendering example of how I would like to be able to model 2d sketches. 

[g-andresen]

Hi,

Can you show a sectional view of your design?  — better: upload your design*

I think the bent parts could be created in the sheet metal workspace and others as solid.

günther

* file - export - save LocalTalk as f3d - attach to your next post

[HughesTooling]

Was the part modeled in Fusion and are you going to use Fusion for the CAM work?

Mark

[davebYYPCU]

There is not much to change from your current method, most of the plates in that example are on one of the 3 origin or offset planes with one slanted plate to finish off.

For that example I would use an origin plane for mirror for the left to right, draw one side and mirror it in place, then construct the crossing pieces.  I make the parts with the tabs with sketches, then later Combine Cut the slots.

Export the faces of each plate with the DXFer plug in to one dxf file.

Better to export and attach a file, so we can point you in the right direction.

Might help...

[Anonymous]

That particular example is not my work so I cant show anything for that one but I will post one of mine in another reply below. 

[Anonymous]

That particular example is not my work so I can not speak on that, but everything I am doing will be done in Fusion and I will be using CAM in Fusion as well. 

[Anonymous]

Thank you Dave. You seem to be keen to what I'm trying to badly explain. 

When you say to mirror the sides, would I mirror them then offset one so they have the spacing I need between them, then construct the center sections? If so what should I be looking up to learn how to accomplish that?

I think I understand what you're saying with the Combine Cuts, is that a command within the program?

DXFer? 3rd party Add In?

I've attached one of my files that I've been working on. It is different from the above posted example as that is not my work. The rendering I've added for this one is also not my work but is a close example of what my finished product will be.

[HughesTooling]

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@Anonymous wrote:

That particular example is not my work so I can not speak on that, but everything I am doing will be done in Fusion and I will be using CAM in Fusion as well. 

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If you're going to use Fusion's CAM I'd look at using derive to create an assembly laid out flat and machine straight off the bodies with no sketches at all. 

You'll need each part to be a component, derive them out to a new design and position with joints so you have precision and easy to edit. Use derive from the create menu to export out to your CAM assembly file, in that file you can edit the derive to add more components if needed.

Mark

[HughesTooling]

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@Anonymous wrote:

Thank you Dave. You seem to be keen to what I'm trying to badly explain. 

When you say to mirror the sides, would I mirror them then offset one so they have the spacing I need between them, then construct the center sections? If so what should I be looking up to learn how to accomplish that?

I think I understand what you're saying with the Combine Cuts, is that a command within the program?

DXFer? 3rd party Add In?

I've attached one of my files that I've been working on. It is different from the above posted example as that is not my work. The rendering I've added for this one is also not my work but is a close example of what my finished product will be.

---

If you want an example using derive can you attach your 3d model as an f3d. You might need to modify your workflow if you're not following Rule #1 and using components for each individual body. An advantage of using bodies and not sketches is the CAM will know which side to offset, with a sketch you'll need to set manually.

Mark

[Anonymous]

Thank You Mark, I will start looking into the derive feature. That sounds like something that may be useful. 

I appreciate your help. 

[Anonymous]

Ahh, see that's where we're back to square one as I have not figured out how to model in 3d, rather only in 2d sketches. But you guys are getting me on the right path as now I'm getting at least the basics of what I need to be looking into in order to model in 3d. Thank you for that link to Rule 1 as I was not familiar with that let alone the difference in component/body/sketch types. 

[HughesTooling]

Have you worked through the tutorials and hands on exercises in the help? Good place to start is sketching.

Mark

[chrisplyler]

I didn't take the time to do alignment tabs/holes, but I threw this together.

I did this with five Sheet Metal components. In each one, I used one sketch and one Flange feature. In all but the flat base, I also used one Bend feature. The bottom riser was just a mirror of the top riser. It took a bit of trial and error to get my bend angles lined up so that everything touches. I sketched/built everything in-place, so that I didn't have to move or joint them into position.

Once the model is done, you can try to CAM each component right in F360, or instead you can make a flat pattern for each component, a second sketch for each component in which you project in the edges of those flat patterns, and Save-as-DXF each of those five sketches to load into your cutter's software. Most software that comes with water jets or lasers allow you to lay out DXF outlines on a sheet of stock. In this way you don't have to CAM it in F360.

[HughesTooling]

If you want to work in Fusion for CAM here's my idea. Parts could be created on the document origin planes and assembled or inplace, I created the second part at the origin then positioned with a joint.

For my idea above you'd need the flat bodies to derive out to another design for layout and CAM. What I've done is with the part finished, flatten then use Boundary Fill set to New Component and the main top component active to create the components for derive. If you need to modify the parts just roll the timeline back before the unfold. I've attached the file if you want to experiment, just use derive from the create menu, make sure you select the components to export not bodies. In the derived design just position the components with joints. If you create a sheet component in the derived design you can position off a corner of the sheet and also select the sheet as the stock in your CAM setup. 

Mark

[chrisplyler]

Sure, that seems fine. Just extra work that doesn't serve much purpose unless you want to create multiple varieties.

[HughesTooling]

He said he wanted to use Fusion for CAM so seems about the only way. But I just remembered the unfolded part is not the same as a flat pattern so it could be a problem with some sheet metal parts. The Fusion team want to make Fusion a one stop shop but not having access to the flat pattern without exporting then importing the DXF is not a good workflow. Some people might want to mill parts out just so they can do it all and there are people building plasma cutters using Mach3 who might not have access to any other software. 

What I show above is totally parametric so change the design, update the derived file and the CAM will all update. I use a similar workflow for mould making. Used to try and use one file for tool design and CAM but found over a certain size Fusion got very laggy, using a derived file for CAM has fixed that problem.

Mark

[HughesTooling]

Here's the page in Inventor's help about the folded part not matching the flat pattern, seems to only apply to a 3 corner bend.

Mark

[chrisplyler]

@HughesTooling 

I wasn't aware of this being the only way. F360 won't CAM a simple unfolded sheet metal component? You HAVE to go through your workflow? You can't just unfold the component and proceed straight to the CAM setup?

[HughesTooling]

You can just unfold but not very easy workflow if you have an assembly. Easier to unfold, copy the unfolded body with boundary fill then refold. Then export all the unfolded components using derive, layout, make as many copy as you need etc. The original master assembly stays assembled and easy to work on and the CAM derived file has a separate layout assembly. All parametric so edits in the main assembly update the derived CAM file.

You could do it all in one file but I found Fusion can't handle lots of components and a lot of CAM data in one file.

Mark

[chrisplyler]

BTW, when made out of 0.10" sheet steel, I would rate that bracket at no more than 200 pounds static to keep a 3x safety factor. Here is 250 pounds on the clevis and it results in a 2.68x safety factor.