Alibre There Eventually - Sort of

Two options there. lets assume you wanted 5mm projection each side.

1. When you create your new part first thing to do would be create a new plane 5mm from the side of gear A. Next draw your circle on that plane. Then extrude that circle and use "to geometry" selecting the far side of gear be as the target geometry and add a 5mm offset.

2. Create the shaft as two end to end cylinders. Draw a circle and extrude to geometry of gear A with 5mm offset. Then draw the same dia circle again but extrude to gear B again with the 5mm offset

I am flummoxed by the idea of creating a part in an assembly, ie, the shaft in an assembly of gears. How does one then create a 2D drawing of the shaft that doesn't exist as a seperate part?

I prefer to create seperate parts, that represent the parts I wlll actually make. When creating a part I don't sweat over dimensions initially. Just create all the features I need to create a part that is topologically correct. I can then go back and add dimensions.

Assemblies are created from individual parts, using constrains as needed. Just as one would build the physical item. I only use constraints that are strictly necessary. Not only is an assembly used to make sure holes in mating parts line up for instance, it is also used to make sure that parts fit together and move correctly when the assembled parts move, as they would in reality. Like this assembly of the motion work on my traction engines:

I tend to design gears complete with accurate tooth forms. Here is a bevel gear model:

An assembly to check meshing:

And reality after CNC machining:

The bevel gear PCD is 1" at the outer end.

Andrew

Alibre Atom is for basic CAD work on a basic computer, my own unit is a 2008 Windows 7 unit

Total cost 250, plus 50 for a decent graphics card

Are you by any remote chance showing us what £2000 of CAD on a workstation costing thousands can do?

Just one of those bevel gears would have my poor computer stuttering to keep up

Andrew, the shaft does exist as a separate part.

If you read my description when in the assembly screen you click "new part" which is next to insert design that you would usually use to bring in separate parts.

You will then find you have the usual screen you would be using to model a separate part but also have the assembly "greyed out" so you just carry on drawing your new part but can make use of any other features of the assembly as reference points. When you then go to save you get a box come up that allows you to name your new part EG "gear shaft" and that will be stored just like a part created individually so 2D drawing easy to produce in exactly the same way.

For example I could do the steam chest cover as my new part, making it's edges co-linear to the sides of the cylinder and using the stud hole pattern of the cylinder to position the clearance holes. Now the god bit is that if at some time you alter the cylinders O/A size or the stud positions then the cover will automatically get updated

I was commenting on the description by Nealeb. Of course it is entirely possible that I have misunderstood the method.

Andrew

Example here for anyone else interested. At the end you can see how the part created within the assembly is saved separately and a 2D drawing of just that part done. Also you can see that when I add 15mm to the width of the gear the shaft also gets extended by 15mm to maintain the 5mm projection each side.

Like Andrew I don't do it that way much but each to their own

Another example of how it could be used is if you have a number of gears and shafts then the casing could be created using the gear shaft positions from the assembly and if you wanted say 2mm clearance around the gears within the casing then that could be done. If you change a gear tooth count then the PCDs will automatically update as will the cavity within the gear casing to accomodate the new gear's OD.

Edited By JasonB on 02/08/2023 10:43:39

Jason -

I see. I need add its own origin plane.

However...

Andrew -

Your question raises something I had not realised; that a shaft created by extruding it through an existing part such as a gear might not be a discrete part (in CAD terms). Would it be an extension to that part?

What though if the shaft is extruded through a matching hole in the existing gear, without using the "New Part" tool? That is what I had done: viewing the face of the wheel in 2D, adding a circle to the same diameter as the hole then extruding it.. Once I found how to do that: it is not so obvious when the drawing is an Assembly not a Part.

I experimented.

That works!

First I tried to move it. I could not despite making a very fancy symbol in bright colours appear. (I have not grasped that Component Placement tool).

Then I discovered the extrusion was listed in the index down the left-hand side as a "New Part", and because I had saved the whole "New Assembly", the shaft was saved as "New Part (1) " . Not only that, I managed, though did not save, a dimensioned, orthographic drawing of it.

So that way round does give separate parts.

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You mention one advantage of Assemblies is ensuring aligned holes, e.g. for screws, do align. Is there any way to leave the holes off the Parts to start with, then extrude them through both Parts in the Assembly? Sort of modifying the Part from the Assembly, not modifying the Assembly by modifying the Part?

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Though if I could ever to learn Alibre Atom to anywhere near the level you show there, I think I'd still be wary of trying to generate components in that way, at least above simple sub-assemblies.

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[Drawing even spur gears to full form is too advanced for me, but anyway my mathematics is too weak for designing gears and I have no CNC machine-tools! I'd have to modify commercial stock gears for bevel drives.]

If you reference drawing 1 properly and use the same xyz plane arrangement for drawing 2 then you can copy/paste your holes straight over to the second part from the sketch in drawing 1

Its part of thinking ahead and setting the job start-up properly, use the grid and be aware of which plane each part is being drawn in

Can save a lot of time and effort later on in a build, it all drops into assembly facing the right way

If you have an odd number of holes in a circular arrangement put your first one at 12 o'clock and do a circular repeat

Edited By Ady1 on 02/08/2023 11:14:07

Nigel,

Is there any way to leave the holes off the Parts to start with, then extrude them through both Parts in the Assembly? Sort of modifying the Part from the Assembly, not modifying the Assembly by modifying the Part?

In the 'Expert' level of Alibre Design it is possible to create 'assembly holes' - think of 'match drilling'. As with all things there are pros and cons to this method.

Even in Atom3D, you can 'project to sketch' the edges of holes in one part into another part that you are creating or editing in the assembly. This creates an 'inter-design relation' so future edits of one part will update the other.

Drawing even spur gears to full form is too advanced for me...

In Pro and Expert levels of Alibre Design, there is support for scripting, which includes a spur gear generator (it is set up a bit weirdly, but I have some modified versions which may be more useful).

Also (and I just checked that this does work with an Atom3D licence) - an Alibre user has programmed an add-on which produces spur and helical gears as well as as cycloidal gears - it does all the maths for you as well as the modelling. Installing the add-on is not complex, but does require familiarity with copying files into program folders in Windows. If anyone is particularly interested, drop me a PM in first instance.

Even though realistic or even 'correct' gears are possible - they will require a fairly good PC spec to avoid making the system very slow to respond.

Placement of any hole depends on the rest of the design. No good putting your first hole at 12o'clock if you have a steam engine cylinder with the steam passages at 3o'clock unless you want a stud cutting into the passage. In a case like that first hole may want to go at 6o'clock or enter a specific angle.

You can't extrude into another part within the assembly only the one you are creating or editing .

You can copy and paste the hole pattern as ADY says but beware that both part swill show the same diameter rather than one clearance and the other tapping size

Or you can draw them on the second part and set their position to be concentric to the holes in the first part in the assembly then if you change one layout the other will change with it and you can size each set of holes to suit.

Andrew - I didn't mention the "create a new part in the context of an assembly" mainly to simplify what was turning into a full-on essay rather than a quick pointer! I think it has been adequately covered in subsequent posts but I realise that it might not be obvious as a technique. I use it a lot. Clearly, once you have that separate part in its own file you can create 2D drawings in the usual way which will include all the dimensions you choose including those "copied" from the parent assembly. As I often go straight to CNC, I often don't bother with drawings unless it's a turning job. Keep thinking about CNC lathe conversion...

I didn't want to add precise details anyway as I'm not an Alibre user - mainly design in Solid Edge and move to F360 for CAM toolpath generation. I think all the general ideas are common to them all but the details differ.

Tried again over the last few evenings but this time slightly more ambitiously - one of my engine's cross-heads.

It's a locomotive type with the small end in a cavity, so I assumed draw it as two halves then stick them together.

The first attempt went all to rats. One half was facing all the wrong ways and I could not flip it over or align it with the other properly.

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I decided where I might have gone wrong, and the second go succeeded that far.

One face has a large hole, opening into the arcuate end of the internal cavity, and on the drawing it was visibly not quite concentric with the arc, but we can't have everything. Much of the time most of the figures were indicating "position not defined" , as well.

'

Then I tried to cut away the ends to form the profile, a sort of portly 'X' shape. That went all to rats too.

I traced the cut-outs on frames of reference-lines, one plotted at each end and made symmetrical about the centre-line by dimensions (must be an easier way).

Then the two halves of the assembly stayed as separate entities so the Extrude Cut tool would work only on one and I could not make it work on the other.

Surely it's not necessary to plot completely the same geometry four times, twice on each half, either.

'

By now I had four drawings.

They were the basic rectangular block with the rectangular guide-bar channels and a rebate for the central plug that holds the gudgeon-pin. That was fine. I think. From that base drawing, the two hollowed-out halves; possibly on the correct planes (the first attempt was all over the shop). Finally, the failed assembly.

I might have had the order of creating the drawing all totally wrong: e.g. should have made the 'X' shape on the basic block. The piston-rod spigot was to have been the last operation. Didn't get that far.

Obviously far too difficult !

Gave up.

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Though of a real thing, I did not need draw it except as just a CAD "exercise" .

An expert would draw it in twenty minutes, then easily incorporate it, twice, in a 3D GA of the whole engine, all parts correctly placed and aligned.

'

Besides, I have already made the two real cross-heads, from their raw casting pair bought from M.J.Engineering at a model-engineering show. I'd spotted them in the waifs-and-strays tray, and a quick measure at the sales-stand showed they'd do! They look as if intended for a 7-1/4" g. locomotive. I machined them from a directly-orthographic drawing in TurboCAD.

There's only one basic route, and there aren't any shortcuts

All you're doing is spending vast amounts of time exploring all the unmarked shortcuts

As the cross head is a single part it should be modelled as a single part not an assembly of 4 parts.

If it is more or less symmetrical then the MIRROR tool is your friend, just draw 1/4 of it and mirror in one axis, then select the original 1/4 and the one you just mirrored (select all) and mirror that about the other axis.

If there is a bit less symmetry then sketch a rectangle of the O/A size and then sketch shapes to cut out mirrored about the ctr line.

Finally add non symmetrical items like pin hole etc.

Nigel,

"and on the drawing it was visibly not quite concentric with the arc, but we can't have everything."

You can apply concentric constraints within sketches - either between items in the same sketch, or between an item in the sketch and an existing 3D edge

"I traced the cut-outs on frames of reference-lines, one plotted at each end and made symmetrical about the centre-line by dimensions (must be an easier way)."

Yes there is - use symmetric constraints in the sketch. Or mirror the 3D feature once produced. Sketch Mirror is also possible, but has some disadvantages.

"Surely it's not necessary to plot completely the same geometry four times, twice on each half, either."

As Jason has mentioned there is a feature mirror tool. In some cases a feature circular pattern can be an alternative - depends rather on the detail of the part.

Quick example of a cross head. For the basic shape I use Mirror for the 2D sketch. For the grooves for the guides I mirror the feature that cut the first one. You can also see at the end where I edit the basic shape then the groove width that I only need alter the one dimension but the changes are mirrored too.

You do need to think about where the lines of symmetry go before you start so that your initial sketch is positioned correctly to the axis it will be mirrored in. Though for more complex items you can add additional planes, axis or guide lines to mirror about.

Thankyou.

Yes, my cross-head is much the same shape as that.

I was trying not to do anything I'd not done before, but could not see how to create the internal cavity except as a hollow in the surface of each of two identical parts. It is not a nice easy shape but has two sides that converge inwards to be tangents on a curved end wall.

Even making that bit was not easy. I could not work out whether you pick the Tangent Constraint then drag the line from the corner to the circle, or the other way round, or what; so when it did work after numerous attempts I had no clear idea what I had done right.

I thought there should be a "Symmetrical Constraint", or something like it, but failed to find one that offered what I wanted: a single line placed centrally across an axis. So I had to resort to very roundabout ways. The little instruction on the command labelled "Symmetric Constraint" is about two separate objects. The nearest alternative, Midline, didn't seem the right choice either.

Then putting the halves together was a nightmare. I had to delete both Parts and re-draw them from scratch to make it work.

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I'm not sure how you meant an assembly of four parts to that stage. It was two parts. I had four drawings, but the first was to generate the two halves, drawings 2 and 3 were the two halves, then drawing 4 was the Assembly of Parts 2 & 3. My comment about four repeats was of the construction to make the corner cut-outs.

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Ady -

I know there is only one basic route, as with any software. I am not trying to "explore" short-cuts that probably don't exist anyway, but trying to use it correctly - or at least as seems to work. Sometimes it takes me so many attempts that I don't know what I did that was finally right.

I doubt I'll ever be able to make more than very simple arrangements of a few simple parts with fine details omitted. Never a 3D CAD GA of an entire machine.

The cavity is simply a sketch on the central plane that is then cut with the extrusion set to "mid plane"

Draw the circle either allowing it to snap to the central point or rough position and then apply a concentric constraint.

Draw a rough line and then make it tangent to the circle add a vertical line so the sketch can be closed once the lines have been mirrored

You can see how Jason drew the original block in the smartest position, thinking ahead

But it's still too advanced if you can't do simple plans yet Nigel

Nigel,

I could not work out whether you pick the Tangent Constraint then drag the line from the corner to the circle, or the other way round, or what; so when it did work after numerous attempts I had no clear idea what I had done right.

After selecting tangent constraint, follow the on screen hints at bottom left of the Alibre Window - you do not drag, you select in order the items that the constraint should apply to. Ideally the first selected item should be the one you do not want to move.

I thought there should be a "Symmetrical Constraint", or something like it, but failed to find one that offered what I wanted: a single line placed centrally across an axis. So I had to resort to very roundabout ways. The little instruction on the command labelled "Symmetric Constraint" is about two separate objects. The nearest alternative, Midline, didn't seem the right choice either.

You should have applied symmetric to the END NODES on the line, about the central axis. I.E. select symmetry tool, click the symmetry axis, click one end node, then click the other.

It might help us to follow along if you don't use the term 'drawings' to mean everything. In Atom 3D there are 'sketches' - these are profiles and paths which are used to help define 3D features in 'parts'. Parts are saved with the extension AD_PRT

The 'parts' get combined into an 'assembly' if required. Assemblies are saved with extension AD_ASM.

'drawings' are conventional manufacturing 2D drawings, which are produced semi-automatically from your parts or assemblies. 2D Drawings are saved with extension AD_DRW.