Alibre There Eventually – Sort of

[Anonymous]

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

Andrew

[JasonBModerator @jasonb]

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

[Nigel Graham 2Participant @nigelgraham2]

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.]

[Ady1Participant @ady1]

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

[David JuppParticipant @davidjupp51506]

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.

[JasonBModerator @jasonb]

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.

[NealebParticipant @nealeb]

Posted by Andrew Johnston on 02/08/2023 10:33:13:

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

Andrew

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.

[Nigel Graham 2Participant @nigelgraham2]

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.

.

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.

[Ady1Participant @ady1]

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

[JasonBModerator @jasonb]

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.

[David JuppParticipant @davidjupp51506]

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.

[JasonBModerator @jasonb]

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.

[Nigel Graham 2Participant @nigelgraham2]

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.

[JasonBModerator @jasonb]

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

[Ady1Participant @ady1]

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

[David JuppParticipant @davidjupp51506]

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.

[JasonBModerator @jasonb]

Posted by Ady1 on 07/08/2023 17:04:11:

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

I would say correctly placing the initial sketch is a fundamental requirement for any part and should be considered from the earliest stage of learning CAD and not something just for when you have advanced up a level or two. Be that drawing something Nigel has in his hand like the crosshead, a part yet not made or modelling parts from an existing 2D design.

[Nick WheelerParticipant @nickwheeler]

Posted by JasonB on 07/08/2023 18:32:23:

Posted by Ady1 on 07/08/2023 17:04:11:

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

I would say correctly placing the initial sketch is a fundamental requirement for any part and should be considered from the earliest stage of learning CAD and not something just for when you have advanced up a level or two. Be that drawing something Nigel has in his hand like the crosshead, a part yet not made or modelling parts from an existing 2D design.

It's also the bit that experience of traditional drafting ought to help with. Weirdly it's the people who don't have that practice that get on better.

[Nigel Graham 2Participant @nigelgraham2]

Jason –

That is as I was trying to draw the cross-head, cutting the cavity to mid-depth on the half. I was going to add the piston-rod connection after assembling the two parts.

I think the bigger problem I had was not appreciating how the sketch would develop, so not planning how to draw the whole thing.

.

Nick –

I have often read this about people whose manual draughting experience makes it harder to learn CAD. I doubt it is true generally, but it could well be true of some. I'd have thought it gives the advantage of knowing engineering drawing as such, but there is the point that most manual drawing is orthographic. You might make a rough freehand, pictorial sketch of the item to start with, but draw it formally in 2D.

Perhaps trying to transfer from one make of CAD to another would be harder.

[NealebParticipant @nealeb]

One reason the 2D to 3D conversion is tricky is that you have to remember that in 2D typically we are preparing engineering/manufacturing drawings; in 3D a sketch is representing some design aspect without any regard for manufacturing. Yes, it has to be "manufacturable" but we don't do things like always dimension from a common reference and we do use constraints like "align with centre" and "make symmetrical".

One of these differences alluded to in the last few posts is an example. When creating a sketch, I often do not try to create a feature exactly where I want it. I create it close to the required position and then add constraints to get it into place and make it stay there. For example, this evening I was drawing a rectangle with a hole in the centre. I drew the rectangle roughly the right size, then edited the dimensions of the sides to make it exact. Then I drew a circle somewhere near the centre, added a dimension to specify the diameter, then applied constraints to align its centre with the centres of each side. My sketches are a bit back-of-envelope while I'm creating them, then I apply constraints (where I can) and dimensions (where I have to) to get it exact. It's a different approach to the way I drew in TurboCAD, for example. In Nigel's example, I would have drawn my line somewhere near the circle, then used a tangent constraint to force it into place. Then a coincident constraint to lock the other end of the line to the line representing the end of the crosshead, and a dimension to get it the right distance from the edge of the crosshead. Quicker to do than to write! But it does need a shift in approach compared to drawing-board techniques.

[Nigel Graham 2Participant @nigelgraham2]

Just finished trying to draw that blasted cross-head again.

This time starting as a half-thickness slice with the end cut-outs. The really awkward bit, taking several goes, was making the halves of the guide-bar channels. I doubt I used the most efficient methods but the two copies – front and back – came out as I wanted, complete with the front one's rebate and four screw holes for the cover.

I placed these four little circles on the corners of a temporary rectangle set by dimensions: I still can't see any other way to make polygons concentric with each other. Maybe there isn't.

The basic shape was not centred on that default grid on the screen so I had to set vertical and horizontal reference-lines. They obligingly gave themselves a node just a little way up the vertical one, and very close to the screen node, making placing the big central circle on their intersection a bit tricky.

So far so good, only I could not foresee that when I collected the rear slice Part for Assembling to the front, it would appear inside out and backwards.

Somehow, I turned the back half so its cavity faced the anchored front half as it should, but it was still wrong. Taking the fixed front half as open towards the imaginary crankshaft, the back half pointed to the cylinder so needed rotating 180º around the gudgeon-pin axis, called ' Z ' on the screen.

I tried everything likely I could find, and on all three axes. Nothing worked.

I returned to its Part sketch – even less help there.

Closed Alibre with its four new files: the basic 'X'-shaped half-thickness slice with its guide-bar channel halves, the right front half, the wrong-way-round-both-ways rear half, and the useless Assembly.

Hopeless……

[JasonBModerator @jasonb]

Why did you still do it as a group of assembled parts I wonder if it is worth answering soemtimes.

If you want to do it in two halves than sketch and extrude the half and then simply mirror that extrusion and it will become one part.

There is a drop down arrow below the rectangle/polygon tool that allows you to construct one from it's centre point out which will give it symmetry and the two axis of the 2D sketch

Regarding inside out an backwards, Again just a sin real life mirror reverses things so would have been a way to do it in the assembly.

Flip tool that I have mentioned several time sin the last couple of weeks will solve the back to face and change to face to face

180deg out of position can again as I have said be done by right clicking the part and selecting "show reference geometry" then constraining one of the assemblies axis to one of the parts axis

failing all that if the two gudgeon pin holes were constrained concentrically you could drag one half round with a mouse and then set its final exact position with simple coincedent constraint.

Edited By JasonB on 09/08/2023 07:14:20

[David JuppParticipant @davidjupp51506]

Nigel,

In almost all cases the 'default grid' in 2D sketch mode is nothing but a distraction – I'd suggest turning it off, so that you get a clearer view of the workspace.

Also unless you specifically want to use it for some reason, make sure 'snap to grid' is disabled.

I believe we covered both these points when I did a screen share with you some while back.

 

Atom3D does not have 'rectangle by centre' that Jason mentions – BUT there are ways you can work around this.

• Use symmetry constraints in sketch to make rectangle symmetrical about default axes.
• Add a reference line across diagonal of rectangle, add a mid point node on the reference line – you can use that to fix the rectangle to existing geometry.

There are probably other options depending upon the exact circumstance.

 

Can I suggest that you stop at each of these small roadblocks you hit and submit a query to Alibre support – send in your file with a clear question. Something like 'how do I make the rectangular pattern of circles in sketch 5 be centred on the hole created by Extrude Cut 3?'

Whilst Alibre Support is not a training service, they don't want you to struggle or fail. Don't feel that any question is too basic (you would be surprised at some of the queries that come in).

You can submit support requests at https://support.alibre.com/s/

 

 

Edited By David Jupp on 09/08/2023 08:00:03

Edited By David Jupp on 09/08/2023 08:00:59

[JasonBModerator @jasonb]

Video of how you could do if it initially modelling one half of the cross head firstly by simply mirroring the features down the left side which keeps it as a single "part" and secondly how you could have gone about the assembly using the flip tool to get the two halves face to face and then using constraints to line the two halves up and lastly using the "show ref geometry" to do the same thing. Suggest you try these with the part files you already have.

You will also see that creating the rebate that forms the half guide bar groove is just a simple random rectangle that is then dimensioned for depth and width before being cut.

[Nigel Graham 2Participant @nigelgraham2]

I didn't realise you can mirror a 3D Part, but I did use that for the initial 2D sketch.

If I had made it as a single block I could not have formed its internal cavity, with its odd shape and centring problem.

(It resembles closely the 4MT locomotive cross-heads in photo 189 of Doug Hewson's latest LNER B1 episode, in ME. My source castings may have been for a similar loco.)

'

I made the ledges as you describe, though my first attempt left thin walls along the outside edge. I had to delete them and make new rectangles extended to reference-lines a set distance from the face of the block.

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No Rectangle menu. Not here! Just Rectangle. I've just opened Alibre and one sketch to see.

No arrow, no drop-down menu.

Resting the cursor on "Rectangle", it says only that it creates a rectangle by opposite corners and dimensions. Right-clicking on it says only "Minimise the ribbon" – a strange thing to do.

I drew a little rectangle away from the main sketch and examined that. I found hovering and left-clicking on it is for editing it. Right-clicking opens a menu partly copying the main tool-bar but saying nothing about placing the figure except by direct co-ordinates.

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I had tried to use the Flip tool. I could not make it work! The whole Constraints tool seemed to lock itself into just one way of working.

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Do we even have the same editions of Alibre? Is yours a more advanced version, with more comprehensive tools and menus? (Mine is 'Atom'.)

.

"… worth answering" ? I am very grateful for everyone's help but perhaps I cannot learn advanced techniques such as Assemblies, beyond say, a plain cylindrical bearing-bush in a simple wheel.

If so I can use Alibre only for individual, simple Parts that can be created in one piece with no difficult internal features.

Edited By Nigel Graham 2 on 09/08/2023 09:38:32

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