Fusion 360 help please.

[Dr.Al]

I will look at a different way of sketching, but I can't see how having multiple sketches is going to be easier to build the item. It may just be that I have got DSM too tightly ingrained and perhaps that is harder than starting from sctratch.

There are a few different ways you could make that part (assuming it is just one part and not multiple bodies)

What you've done as a first sketch is a reasonable approach (but certainly not the only one). I thought I'd work through a couple of methods to show how I might do it. I won't use Fusion because I don't like it, but the method would be the same in principle.

For the first method, we'll start by creating a sketch on one of the main planes:

You'll note that there are only four dimensions driving this: the overall box size of 100 mm (with the left side and top side constrained to be equal), the construction box size of 70 mm, the inner circle size and the top-right mounting circle size. Everything else is constrained to be equal to or coincident with something else.

That gets extruded (I went with 3 mm thickness):

I then create a new sketch on the nearest face of the part:

This time, there's only one dimension. I created some construction lines going between the left side and the outside and between the top side and the outside and constrained them to be equal. That keeps the thickness the same, even if I go back to the earlier sketch and make it non-square. I didn't draw the outside box: I just pulled it (referred to as "Convert Entities" or "Use (Project/Convert)" etc depending on the CAD system) from the body.

I then extruded that (merging with the first body):

The same face as before was used for the next sketch, which needed three dimensions:

which was also extruded:

Note that I'm just picking random numbers for the dimensions as I don't know what you're aiming for.

I then span the part round and created a sketch on the back face:

The circles are constrained to be concentric with the bore of the existing part, but I deliberately didn't use the inner diameter as your model makes it look like there's a reduced diameter and I'm trying to match that look.

That got extruded in both directions, 1 mm one way and 40 mm t'other.

Okay, it doesn't look much like yours, but that's what comes from making dimensions up as I go along

This is the method I probably would have used to make it: hope that helps.

I'll post an alternative construction method in the next post....

 

[Dr.Al]

For the second method, I thought I'd start with a much simpler sketch:

I extruded that quite thick:

In some CAD systems, you can also directly insert a cuboid by just giving it the dimensions, but I tend to use a sketch anyway.

I then used the Shell command to hollow it out, with 6 mm walls on the narrow faces and a 3 mm wall on the big face:

Another sketch was made at the bottom of the pocket:

and an extruded cut used to make that lot into holes:

The rest of the process was much the same as before, so I'll stop there...

I hope that was useful. I'm sure there are plenty of other ways you could do it.

There are also things called "Layout Sketches", which are single sketches driving multiple parts in an assembly. I'm not sure they would help with something like this, but they can be useful if you're trying to interrelate different parts.

I'd be interested to see something similar to what I've just done describing your process in DSM. Personally, I hate DSM (not least because of the restrictions on essential things like STEP export), but I understand that you're used to it. Seeing the detailed methodology you use for making stuff in DSM would help us be able to advise on what's different in parametric CAD and why.

 

[ajlelectronics]

Well that is very instructive, thank you. I am struggling now with the insert part, so many I will go back to DSM for now to show you and then have another go tomorrow.

It will start with a full size square of 140mm which is then "pulled" (extruded) to thickness 2mm. Then the inner square of 127mm is drawn, together with the 4mm screw holes and the 2mm thick 100mm OD collar. All the holes can be selected as a set and "pulled" through the material to make a hole. Pulling them in the opposite direction will form columns. The same process is used to form the collar, pulling it away from the surface to create it. There will be a surface in the centre of the collar which needs to be deleted. The surround is extruded in the same manner.

 

[Dr.Al]

Just for fun, I thought I'd show the Synchronous modelling method that Solid Edge offers (as an option). It's worth noting that I'm very much not an expert at this...

In Synchronous modelling, you don't create a sketch, you just start sketching. Here, I've selected the centre point rectangle tool and offered my mouse up to near the centre. I can press F3 to lock it to a plane, or just start drawing and be careful with the mouse (I chose to use F3):

When you start drawing the rectangle, it pops up some boxes, so you can just type in dimensions.

You can add "Design Intent" dimensions if you want, but it's not mandatory and (in Synchronous modelling) it isn't pushed as hard as in "normal" parametric CAD. I'll choose to go with the flow and leave it undimensioned (note that it is the right size as I typed 100<ENTER>100<ENTER><ENTER> so the two sizes are set to 100, even if they're not constrained.

I can then click on the face:

and drag that arrow with the blue ball on it out:

Again, I can type a number in and hit enter and that'll be the length.

In this case, the dimension appears automatically:

I think that, if I had dimensioned the sketch, then those dimensions would be visible too (they can, of course, be hidden).

I've decided that I want to make this box a bit bigger and non-square. I'll make it 120 × 90 mm. In "normal" (ordered) CAD, I'd go back to the original sketch and edit it. In Synchronous mode, I just dimension the things I want to change:

Continued below...

 

[Dr.Al]

I can now use the Shell function (called "Thin Wall" in Solid Edge) to open out the box. Note that Solid Edge doesn't allow different thicknesses on different walls (as far as I can see), so I make it 5 mm all round.

To make the back wall thinner, I just select it and drag the pointer backwards (it gives me the option to type the distance in, so I type 2<ENTER> to move it back 2 mm):

I have to tweak the drag settings as I go to make it cut rather than stretch the whole box:

I can then draw directly on that bottom face:

I can then select the regions of interest:

and drag them backwards to cut

etc...

I'm definitely not as familiar / comfortable with this way of working (I like my fully constrained sketches and well defined order of operations), so I doubt this is a good example of best practice. If you're interested, try googling "Solid Edge Synchronous Modelling": there are loads of videos showing how it works and explaining it much better than I could.

 

[ajlelectronics]

That is very much the same as DSM. I have just been trying to do it, but my brain doesn't want to play. I'll have another go later although you have actually done it the way I was going to in DSM anyway.

 

[Dr.Al]

That is very much the same as DSM. I have just been trying to do it, but my brain doesn't want to play. I'll have another go later although you have actually done it the way I was going to in DSM anyway.

Are you doing commercial stuff? If not, then Solid Edge Community Edition is free (and it's a one-time install that doesn't need a licence to be renewed annually like Fusion does). If you prefer that way of working, then stick it in Synchronous mode and you'll be away. If you ever feel the urge to use conventional CAD methods, then you can switch to Ordered mode and give it a try.

From the webpage (https://resources.sw.siemens.com/en-US/download-solid-edge-community-edition):

 

[Misterg]

Are you doing commercial stuff? If not, then Solid Edge Community Edition is free (and it's a one-time install that doesn't need a licence to be renewed annually like Fusion does)

Does it do 3D CAM? I did have a look at the web page, but couldn't see any mention of it, other than 3D printing

 

[Dr.Al]

Does it do 3D CAM? I did have a look at the web page, but couldn't see any mention of it, other than 3D printing

No idea, sorry.

 

[Dr.Al]

Does it do 3D CAM? I did have a look at the web page, but couldn't see any mention of it, other than 3D printing

Having done a bit of googling, it looks like the answer is no. Siemens are seemingly quite protective of their CAM software so they don't include it in the free version of the CAD package.

Of course, you can always use a different CAM package so you get the advantage of the powerful CAD software that's permanently installed on your PC and just export a STEP file for CAMming. Obvious free choices are FreeMill (part of the Rhinoceros CAD system), FreeCAD (which can do CAD as well, but the CAD isn't that intuitive - no idea how easy the CAM is to use), or even Fusion (just import your Solid Edge STEP file and do the CAM part there).

The latter option might seem an odd choice (why not just use Fusion for everything?), but if you do the CAD work in Solid Edge, then when Autodesk cut the free version of Fusion down even more, you'll still have your models in a fully featured CAD system and you can just switch to FreeMill (or whatever) for the CAM.

 

[Misterg]

Of course, you can always use a different CAM package so you get the advantage of the powerful CAD software that's permanently installed on your PC

Thanks very much- It’s just too convenient to use F360. I probably won’t do anything until / if I’m forced into it though!

 

[ajlelectronics]

I seem to have got a suitable design for the rear section and so now I need to make an insert section which carries the hinged flap and directs the air flow, a sort of triangular shape. External dimensions I suppose are going to be the same as the internal of the base at 127mm, because it needs to fit tightly. I have added the recessed screw holes in order to fix it more securely than the original plastic pips design.

I found that I could sketch inside the recess and then extrude that out, including the location pip slots, which was nice. However that extrusion appeared not to be a separate part, but becomes part of the base. How should I approach that please?

 

[Erie Fred]

Start a new assembly, bring your existing flange in as the first part, locate it at 0,0,0.

Draw the other part, save it as a part, then bring it into the assembly.

Mating conditions to stick them together.

If the second part has features that mate to the first part, leave them out for now.

After mated up, edit the 2nd part while inside the assembly, project the details
from part #1 across into part #2's sketch.

This way, if you modify part #1, part #2 will follow along.

 

[Dr.Al]

The way @Erie Fred has described it is definitely the proper way to do it.

If you want a lazy way, most CAD packages (not sure about Fusion, sorry) allow you to have multiple bodies in a single "part". OnShape actually encourage it if the parts share important dimensions, but I think that's quite unusual (except for "Weldments", which are usually done in the multi-body way, regardless of package).

To do the multi-body way, look carefully at the options when you do the extrude on your second part. I'm not familiar enough with Fusion (have I mentioned I don't like Fusion? ) to know what the setting is called, but there's usually an option not to merge when you do the extrude.

I haven't got Fusion on this PC, but to give some examples from other tools:

OnShape: when you click Extrude you can create a New body by clicking on New:

Solid Edge: when you Extrude you can click on Add/Cut and select "Add Body":

Solidworks: when you do "Extruded Base/Boss", you can untick Merge:

ZW3D: when you extrude, there are pictures showing the different types of merge:

Fusion will almost certainly have something similar.

Once you've got multiple bodies, you can work on them together. When you export as STEP, they should come out as an assembly of two parts. PrusaSlicer can read the STEP file directly.

I'm not sure how Fusion would handle exporting STLs of multiple bodies. OnShape spits out a ZIP file with two (or more) STLs included. You might have to select each body and export separately. Getting out of my Fusion depth here a bit.

As mentioned before, this isn't really the "proper" way of doing it, but it works and will probably be fine for what you're doing. In-context assembly design is quite a bit more advanced.

 

[Erie Fred]

I do it this way, after years, many years of work, of having to always make changes midstream.
Damn customers.

Also, I have found out the hard way, that the longer method i described is better when you need to re-visit the files a year later for changes.
You can clearly see the parts, the mating, the links, etc.

Having to call up some one else's work when done the "tricky slick" way, and make changes, things go sideways real fast.

 

[ajlelectronics]

I found that I could specify an offset for the extrusion to start. I pulled it to 80mm and to close the hole, selected it, right click and delete filled it. So now I have a solid block to fiddle with next session, with the slots in the right place.

Thanks both.

 

[Erie Fred]

I found that I could specify an offset for the extrusion to start. I pulled it to 80mm and to close the hole, selected it, right click and delete filled it. So now I have a solid block to fiddle with next session, with the slots in the right place.

Thanks both.

The slots are linked to the other part ?
Or did you just pull a "blind copy" off of the original part ?

 

[ajlelectronics]

Or did you just pull a "blind copy" off of the original part ?

That.

 

[Erie Fred]

That.

There is no neat way I know to flag the part (change color maybe)
so that you know it won't update when the mating part is changed.
Isn't the part in question a $3 dryer vent ?

 

[ukracer]

To draw that how fusion wants you to draw it you'd draw your base sketch, extrude, then select your new face, create sketch, then draw your next face to extrude, and so forth. you're drawing all sketches then wanting to extrude them all from one sketch.

I now know why I can't use fusion very well. I don't know what the hell you just said then.