Hopeless…Alibre Ass

[Nigel Graham 2Participant @nigelgraham2]

I realiesd I needed make four major changes to my steam-wagon engine:

1) Compound to twin simple-expansion, so I have to make a new cylinder block.

2) Change the connecting-rod centres from 4.5 to 7 then to 6″ centres. (I.e. make a third pair.)

3) Place the crankshaft and main bearings below the engine base-plate, rather as in a car engine.

4) Make a new base-plate as the existing one is too short.

So four new Alibre Atom models: the new base-plate, connecting-rod (badly) and journals (2 sizes plus bushes for 2 of them).  I very much doubt I used the most efficient methods but those are for the experts.

 

Then tried to assemble them. Far too hard.

I needed create the studs to align the journals.

The crankshaft is not truly concentric with the journals.

The connecting-rods arrived upside-down. I took ages to make them point upwards through the base-plate “windows” although at strange angles: “Axis” tool then “Component Displacement” by angle that only worked by including a small linear displacement.

I don’t know how to assemble the big-ends centrally along the pins but that does not matter much. The clearance is tiny.

So far so… good? No – I’d hit the end.

Assembling the cross-heads from their three parts, failed. The parts arrived facing in random directions and every move was just “over-constrained”. I deleted them.

The Design Explorer by now listed six axes and two dozen constraints, excluding all the faulty ones I had deleted. I expect the real Alibre users would knock that assembly off in half that, accurately, in ten minutes. That is NOT a challenge! Anyway, it would only prove my point if anyone did.

 

A complete mess. At least it’s not wasting metal, electricity and time making parts I need replace later, just making useless pictures.

Hopeless….

 

 

 

[JasonBModerator @jasonb]

A few random comments

Conrods arriving upside down. Use a constraint to make the hole in the big end concentric to the crank pin. You can then simply hold the mouse down on any part of the conrod and move it, the big end will stay where it is so the rod just swings round. Until the cross head is in place you won’t have anything to constrain the little end to.

Conrods sideways. Two options one is to select the side of the big end and the side of a web and use an offset constraint entering a distance of half your gap. Right clicking the rod and selecting “show reference geometry” will then allow you to position the ctr line of the rod, probably half the cylinder ctr distance from the mid plane.

Crankshaft concentric to journals. Should just click teh journal surface and teh mating round part of teh rod and us ethe concentric constraint

Cross heads. To simplify things do an assembly of just the three cross head parts. constrain mating faces, concentric holes, colinear faces etc. Save as an assembly and then import into the main assemby.

No need to have added any extra axis. If you have deleted aulty constraints then they would not show in the tree down the left so you can’t have deleted them. Yes the list gets long but by using sub assemblie sand naming some of teh constraints you can keep their number down and keep track of them.

Studs (and other fixings) No need to add these at the moment and nor that important later. If you have the tapping and clearance holes then you just set them to be concentric. Again keeps the list on the left short and if you have a slow computer means it does not have to work so hard.

One other thing I see is that your assembly is not positioned  to any particular axis. I would have started with the base plate and centered that on the ZX plane and anchored the part. That way you have a ctr line running down the middle of teh engine.

[David JuppParticipant @davidjupp51506]

If you need to change things – edit the existing models, there’s rarely a need to make new ones.  This is huge advantage of parametric CAD.

If the existing parts are already in an assembly it will be updated by the edits of the parts.  As long as the topology of parts doesn’t change radically, assembly constraints will still function.

Changing con-rod centres should just be a matter of changing one dimension value and then generate to last feature.

Fix the first or most major part in an assembly so it can’t move (either anchor or add assembly constraints) – that makes adding other parts much simpler.

[DiogenesParticipant @diogenes]

Ha, yes – I made one of these to prop against the monitor stand when I first started, it helps ensure the parts arrive (hopefully) in the assembly space the right way up..

[JasonBModerator @jasonb]

Yes comes back to what I have said before. When you start to draw a new part think of it’s final position and choose your starting plane accordingly. If you look at the parts that make up one of my engines just about all the icons show the part in it’s correct orientation so when added to an assembly you are off to a good start.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou Chaps.

I can usually model individual parts that do not have features like compound angles, curves, pipe forms and helices. I could probably draw many of the simple parts in your screen-image, but not ones like the Cylinders.

It is Assembling anything that is beyond me, either in Alibre or TurboCAD 3D.

Although I try to create each Part to lie correctly when imported, they still drift in like Autumn leaves before settling any old way round.

I may be best leaving that side of CAD for a few weeks before trying again, but might simply need abandon it. I just go round in circles, solving one problem only for others to appear again.

.

Rather than trying to align tapping and clearance diameters I use only the outside diameter for such features, and where necessary, temporarily represent washers to verify fastener widths and clearances. The actual drills and taps instruction can be by annotations. (Apparently, matters like accessibility for spanners have been known to trip up even the professionals. Though this is a road vehicle I am “designing”…!)

I still could not align the bearings to the base without using the studs though. Also as each moved across the screen it rotated in an unexpected way. So each block needed three constraints to place it.

I did constrain the crankshaft’s centre surface to its journal bore but it still shows errors. Possibly, I have not plotted the journals fully in line. One slightly overlaps the edge of the plate so there is an error there, too.

So far that is just fifteen Parts, and six of those are studs represented as plain rods. How many parts in an entire engine, even if I represent only half of the motion-work? All joining each other in quite complicated ways?

I can see the point of making the three-part crosshead a sub-assembly but I expect I would still meet the same problems.

The Base was the first Part in, and is anchored.

.

I know how the Design Explorer records faulty axes and constraints, and I remove those from the list.

.

On modifying parts to new sizes, I tried but could not make that work properly. I might have been trying to change it too much. The Base-plate in that example needed quite a bit of revising.

.

Having established a few more of the smaller components, making them would enable me to verify some of the dimensions to help working out the size and shape of the casing that holds it all together.

 

Incidentally, the heading is actually “Hopeless – Alibre Assembly”. I’d not realised how the titles list would truncate it!

 

[JasonBModerator @jasonb]

OD, clearance, tapping, etc it makes no difference you can just set one hole concentric with the other – no need for the studs.

Th eparts don’t fall like leaves they have the same orientation as when they were created, position is down to where you click the screen.

[David JuppParticipant @davidjupp51506]

“So each block needed three constraints to place it.”

Yes – that it typical to fully constrain any part!

[Nigel Graham 2Participant @nigelgraham2]

Jason –

I thought that should be so but I found it so difficult that I added the studs to help me.

I don’t know what the Parts are really doing but they do tend to twirl round or over, even both. They don’t “flutter” but their native orientations are clearly not that of the assembly, and I cannot see what is happening. Only that they finish the wrong way up or round. I know there is that rotation thing on the Constraints menu but have never made it work, nor known exactly when it can or can’t be used.

 

David –

That’s a relief at least. I thought I was having to use so many constraints to correct built-in mistakes.

[DiogenesParticipant @diogenes]

Nigel, your ‘unexpected rotations’ – is it possible that you could be forgetting to always click the ‘Apply’ button on the bottom of the Constraint Dialogue Box at the appropriate point after defining each particular pair / set of items – omitting to do so does indeed result in (very) unexpected rotations and movements because ‘clicking the next item’ whilst the last constraint instructions are still ‘active’ will often force that item to try and conform..

 

 

[Nigel Graham 2Participant @nigelgraham2]

Thankyou for that tip. I had the impression that if you forget, the tool simply has no effect.

Essentially I was trying to make a block with two holes in it line with the corresponding holes, which would carry studs, in a plate.

I found it far easier to “fit” the studs then constrain what seemed the appropriate hole in the block to one of them. The block would obligingly thread itself onto the stud then rotate around it in the wrong direction.

I assumed this is because any part I bring into an assembly points anywhere but in the right direction.

[DiogenesParticipant @diogenes]

I do as Jason mentioned earlier, first just put a concentric constraint on the edges of the ‘stud holes’ and then either one on a matching edge of the block & base (to pull them together), or I just ‘stick’ the mating faces together, depending on how the parts conform..

[JasonBModerator @jasonb]

Don’t beat yourself up looking to apply 3 constraints to everything as some parts won’t need that many.

Although you do need to set a parts position in three axis using a concentric constraint will actually locate it in two axis so you only need add a second to completely tie down it’s location.

 

Not to confuse you more so ignore this if anyone is an Atom user different versions of Alibre can handle that sort of constraint differently as they have a “fixing” constraint which will both make the two holes concentric and also bring them together all as one constraint, though I don’t tend to use that option.

[David JuppParticipant @davidjupp51506]

If a pair of holes won’t constrain parts together correctly – one common problem is that the hole spacing isn’t EXACTLY the same in both parts.

[Nigel Graham 2Participant @nigelgraham2]

Diogenes –

That’s what I was trying to do, at first.

Last night I tried assembling just the cross-head on a new file of its own. It is a hollow casting with a cover-plate held by 4 small screws between two location ridges, and a central pin. Just three pieces and 4 small screws.

I anchored the body, but the cover went all over the place, dissolving randomly into the casting, raising “over-constrained” errors, etc. Nothing would work. I simply had to close the file unsaved, and Alibre itself.

.

David –

How do you ensure the spacing is accurate enough for CAD – assuming of course not simple typing mistakes that mean the operator makes the two parts differ anyway? I know CAD will round off and display dimensions to the decimal places you choose but works internally to extremely fine mathematical limits. What precision do you need set in the drawing’s properties?

 

[JasonBModerator @jasonb]

You want them to be the same. So enter the same number when modeling the two parts, copy and paste hole locations from one part to the other or model one part using the other as the reference making say the holes in the bearing concentric to those in the plate.

You need to watch how you model individual parts to ensure they match. For example if on your plate you entered the hole centres as 0.625″ apart and when modeling the bearings you set a hole 0.312″ from ctr line and then mirrored it you would end up with 1thou difference.

Not sure if Atom has it but you can set some play in other versions of Alibre but better to model them the same and then it’s down to the machinest.

If you want to send me those cross head parts I’ll stick them together for you, just remind me what version of Atom you are using eg 26, 27, etc

[David JuppParticipant @davidjupp51506]

Nigel,

You just have to be consistent.

So if modelling directly – just take care to type in the same numbers.

If using ‘real time dimensioning’ – take care not to disturb the mouse whilst entering values – mouse movements will alter the value that was just typed.  Much of the time I avoid real time dimensioning, but it can be a time saver.  The separate dimension tool is more robust.

You can type in more decimal places than the display precision currently selected – the displayed result will be rounded.

If things don’t seem to work when they should – set units precision to maximum (6 decimal places) – that often reveals minor differences when using the measurement tool to check spacings.

Anther thing I’ve seen when diagnosing assembly constraint issues – a part that looks rectangular actually has a corner angle very slightly off from 90°, so the parts can’t fit perfectly (in real life you’d never notice the error).

You can potentially make sure spacings match by either

• Use one part as the ‘master’ and use it to drive features in the mating part.
• Use a spreadsheet to drive more than one part from a single list of dimensions

These have benefits, but also introduce their own complications – so may or may not be for any particular user.

 

If you do find that dimensions don’t match when they should, it is possible to edit the value in one or other part to make them match.

[Nigel Graham 2]

On Nigel Graham 2 Said:

How do you ensure the spacing is accurate enough for CAD – assuming of course not simple typing mistakes that mean the operator makes the two parts differ anyway? I know CAD will round off and display dimensions to the decimal places you choose but works internally to extremely fine mathematical limits. What precision do you need set in the drawing’s properties?

 

You don’t, you let the computer do it. This means thinking in a CAD appropriate manner, not drawing on paper. So you would align your cylinder covers using the bore centres, and use the hole function to apply the holes to both components at the same time. That’s assuming that you didn’t design the cover in place, which makes everything easier.

[Nick Wheeler]

On Nick Wheeler Said:

…, and use the hole function to apply the holes to both components at the same time. 

A problem for Nigel is that Atom3D doesn’t support that particular workflow.  It doesn’t have ‘assembly features’.

[David Jupp]

On David Jupp Said:

On Nick Wheeler Said:

…, and use the hole function to apply the holes to both components at the same time.

A problem for Nigel is that Atom3D doesn’t support that particular workflow.  It doesn’t have ‘assembly features’.

Then he would layout the hole pattern and apply that separately to the relevant components after assembling them.

The thing to note is that parts should be assembled using the features that are most relevant: I would use the centre(both for the circumference and the length) of a big-end bore to the same spot on the crank pin to attach a conrod, which means that it doesn’t matter how the part is aligned before assembly. No rotational alignment is necessary because the rod-to-piston-to-bore joints will take care of that.

[blowlampParticipant @blowlamp]

Nigel.

I admire your determination, but think that after all the time you have spent struggling with the fundamentals of Parametric CAD, you might be better off exploring a Direct Modeling CAD package.

Could you list the main requirements that you need from CAD for it to work for you?

Martin.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou for the compliment Martin, though dogged insanity would be a better description.

It’s not whether CAD can work for me. It would do that as much as it does for anyone else if I could drive it properly.

I’ve just spent at least an hour trying to make sense of what should be a simple assembly – a locomotive-type crosshead comprising the main body, a cover-plate and a pin, plus a few fasteners.

As well as struggles with the CAD methods, I found I can’t even measure two bits of metal. I discovered the models for both the body and the cover contained serious measuring mistakes that made them totally un-matched.

I deleted both drawings and re-drew the cover. That was easy but I have not created a new model for the crosshead body. That could take me at least three hours, thanks to its fancy shape needing a lot of geometrical construction.

Since the real pair are made I’ll represent them on the general-arrangement by rectangular blocks.

…..

Main requirement for CAD? Being easy to use – but the more useful it is as a design aid the less easy it will be.

I don’t want to “explore” failing at yet another CAD make, but I use a rather inefficient work-round using two different ones to overcome being unable to use 3D CAD for assemblies.

I can though, model fairly simple, single parts in 3D using Alibre Atom; and make assembly-drawings using TurboCAD in its 2D mode.

Unlike Alibre, TurboCAD gives a full 2D / 3D choice, so although both programmes’ 3D assembly methods are beyond me I can develop general-arrangements directly as orthographic drawings.

On the other hand, Alibre Atom 3D is often quicker and easier than TurboCAD for drawing single Parts, and printing dimensioned workshop drawings from the model is certainly simpler than TC’s convoluted counterpart.

 

So I use whichever is the better for the task and according to what I am able to do with it.

 

 

[blowlampParticipant @blowlamp]

Nigel.

There are no assemblies or constraints in many Direct Modeling CAD apps, so that would take a burden off you straight away.

As you are finding, Parametric CAD  has to be ‘driven’ correctly if it is work as expected, but Direct Modeling CAD cares not at all about the location and relationship of the parts within the drawing. However, it’s very straightforward to make all sorts of perfect alignments between components which are every bit as good as those in a Parametric Modeler – only it’s not done automatically.

I use a Direct Modeler myself and can draw pretty much anything I’ve seen done on here and I enjoy the freedom it allows.

 

Martin

[JasonBModerator @jasonb]

The down side of Direct Modeling in Nigel’s case would be that if like his crosshead he makes an error modeling the first part then all the subsequent parts based on its geometry will also be wrong.

At least as David has said if a part won’t assemble it is quite a reasonable bet that it is due to one or both not matching which as in Nigel’s case seems to have shown up his original error.

Nigel, how many more times does it need to be said. Don’t delete and start again, just alter the part to correct any errors.

I suspect one of Nigel’s other requirements from any CAD package would be good support. We know he does not like watching video so do the other options have good support, will they have staff members willing to spend as much time as David has done on the forum and also with one to one tuition? Also a userbase that is also willing to help him like myself and others have done.

[blowlampParticipant @blowlamp]

Jason.

 

Far be it from me to try and read Nigel’s mind, but it seems like Parametric Modeling might not suit his natural way of working and despite his best efforts with at least two modelers of this type still can’t make reliable assemblies.

When you wrote “Nigel, how many more times does it need to be said. Don’t delete and start again, just alter the part to correct any errors.”, I think you showed that Nigel’s inclination is to restart his sketches and that inclination would be a better fit for the Direct Modeling approach to designing his wagon.

Nigel has tried these two well supported CAD apps, but still appears to be be finding it difficult to progress. I suggested that he tries Direct Modeling on the basis that by the time he really understands how to ‘drive’ a Parametric Modeler, he could have redrawn his parts a thousand times in a Direct Modeling app. 😉

 

Martin.

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