Had Another Go

[Nigel Graham 2Participant @nigelgraham2]

Thankyou!

I went back to the original and tried it. I rounded off the outside edges successfully, but found with the inner ones it would remove rather than add “metal”, rounding both entities’ edges to create a peculiar cut-away effect. I took this to be because here, an edge of one entity meets a face on the other, as two separate objects.

Not really important though, just a minor finishing-touch. It was difficult enough and took long enough, creating the main model. I suppose it would have been more efficient to have modelled a quarter-section of the three channel parts, reflected it twice to the overall shape then added the angle-piece. I can see why that Sweep tool exists for extrusions not parallel or perpendicular to the main axes, but cannot operate it.

The ends of the cross-pieces don’t meet the sides very well. I had to use one corner on each cross-member to locate the side wall so there are tiny triangular gaps in there. Then having extruded the primary sketch realised I’d put the angle-iron cross-piece at the wrong distance and had to remove it by extruding a rectangle through it, and add a new one at the right spacing.

I found that sketch-verifying very frustrating because it lists your mistakes but does not show where. Some are fairly obvious on an enlarged view, but others really are hidden. The inviting button called “Analyze” doesn’t seem to do anything, not in Alibre ‘Atom’ anyway. I expect it does in the higher-power editions.

…

I had first tried to assemble this frame from the set of parts I’d drawn, but failed very quickly.

[David JuppParticipant @davidjupp51506]

Nigel. If a feature is in the wrong place, you don’t need to cut it away – instead either delete the feature in the design explorer, or edit the defining sketch to correct the position.

The analyze tool will show you where particular errors are.  Select any error in the list, and the location will be highlighted.  Not 100% perfect, but it can be very helpful.

[Nigel Graham 2Participant @nigelgraham2]

David – the wrongly-placed piece was a part of the sketch itself so I could not delete it on its own, but I could not work out how to edit it either.

I was hoping the analyser would highlight where the errors are but it didn’t, so what do I need do?

I tried switching off 3 of the 4 types listed and pressing “Analyse” but that didn’t seem to make any difference. I think some of the errors were so tiny they were invisible, hidden by the line thickness and the black dot.

The “Heal” button is definitely off – low-lighted.

I cured some by extending the outlines beyond the corners to meet temporary external lines, then trimming them back.

[JasonBModerator @jasonb]

When you use analyse it will list the errors, click on them one at a time and it highlights them in red. Work your way down the list. Usually two lines not meeting or a line overlapping.

To edit a sketch You should right click the sketch number down the left size and select edit. Then go upto the top and select “trim” you then click on any of the lines or curves that you don’t want and it will remove just those leaving the ones you want. Not that if a line crosses another then the trim tool will only trim upto that crossover so you could have missed a tiny part that is still on the screen but hard to see until analysed.

Your unusual “cutaway” rather than a fillet sounds like you have sketched it as separate parts to make up the C section and they are not really touching even if they may at first look like they ar eon screen so the tool is rounding over an edge rather than filleting between a solid.

[Nigel Graham 2Participant @nigelgraham2]

Ah – click on the errors. I’d not known that. Thankyou.

I think the faults were mainly lines not meeting properly, though I also found a tiny fragment of overlapped line almost hidden in the surrounding, correct lines. I needed enlarge the image considerably to see it.

Yes- I had made each C-section as three separate parts. That’s why the complete model has so many extrusions. The line’s screen image is wide enough to be visible, so probably hides any tiny gap. Worse of course where I made the second one of each pair of flanges by merely tracing the one beyond it.

 

Next thing is to try to print it but shrinking it enough to fit an A4 sheet means it may not be very useful. This is where I needed the A3 printer I’d bought for using with CAD, but which had broken down and could not be repaired.

Though a single Part to concentrate on the space in the middle, its sides extend far enough forwards to nearly meet the boiler brackets, and to include the position for the steering column and gear-box. They also reach back enough to cover the nominal location for the radius-arm joints, on plates below the chassis, and on the centre-line for the final-drive shaft.

It’s quite a busy area!

…

I have a collection of lengths of extrusion models for this frame, each length as a Part, for Assembling into the complete frame, but when I tried putting them together, I couldn’t.

[JasonBModerator @jasonb]

Yes you often need to zoom in to see the error but at least by clicking them on the list you will know to look at the red highlighted area.

When you are making a shape up from separate parts you can use the “–” co-linear constraint to line your new sketch to an existing edge. Or use “project to sketch” but that is a bit more involved.

Re printing on A4 you can set the scale of your part bigger than will fit within the blue eboundry of a A4 sheet and then move it about after printing the first position so you could end up with four A4 sheets each with a 1/4 of the  drawing on them that can be taped together. No different to how you may have used the works photocopier in the past.

I did not save a drawing I used last week but will take a photo later to show what can be done for home use.

[Nigel Graham 2]

On Nigel Graham 2 Said:

[…]  Yes- I had made each C-section as three separate parts. That’s why the complete model has so many extrusions. The line’s screen image is wide enough to be visible, so probably hides any tiny gap. Worse of course where I made the second one of each pair of flanges by merely tracing the one beyond it.

[…]

That takes me right back to when I first used Autocad

Wherever possible [i.e. at every available opportunity] let the ‘machine’ do the work of finding and connecting endpoints, tangents, etc. etc.

It will be happy with its own work !

Way back in v2.18 for DOS Autocad was working to 14 places of decimals, and would not tolerate tiny gaps between ‘manually-drawn’ lines.

From what I have seen [in the previously-recommended Video] Alibre Atom provides excellent tools to assist you in the crucial sketching process.

MichaelG.

[JasonBModerator @jasonb]

So here is an example of getting a large part onto a sheet or more.

This shows the base and capital details of some columns I was machining last week. If I had put the whole column on the A4 sheet I would have to have printed at 1:1 scale which would not have been ideal to see the dimensions on the mouldings. Could have done a detailed view in this case but for ease and what Nigel wants I just brought in the column twice and positioned them on the screen with just the bottom of one and the top of the other within the blue page boundary and printed. Think they are at 5:1

For Nigel’s chassis the program will assess the size of the part and the paper size and automatically scale it to fit. This can be changed quite easily so I went from 1:19 to 1:1. As you can see most of it is outside the blue boundry which is the A4 sheet. But if that is printed and then the chassis dragged around until you have the 4 parts of the tapered  section all within the box one after the other you will then have the chassis on four sheets that can be taped together. Just like moving an A2 printed plan about on a A4 photocopier

On Screen in Alibre

 

Printed to PDF in this case

I did add the ctr lines to make taping them together more accurate.

[Nigel Graham 2Participant @nigelgraham2]

Michael –

Yes, I know CAD does work to as many places of decimals as the computer can spare, and expects lines to meet properly.

This caught me out when I first took it up, with TurboCAD: I drew a cross-section but could not cross-hatch it. I’d tried to join the vertices visually, not knowing I had to help the system to close the shape as a “polyline”. (I have subsequently exploited this to create a thin-walled, open box as an extruded, thick line. I’ve not tried similar in Alibre, which will say the sketch is not closed; “Open Loop” error I think.)

 

Jason –

Yes, I could certainly do that.

When I took my A3 printer for repair the dealer was unable to obtain spares for it – out of production. He suggested if I want proper prints larger than A4, doing what he does, by taking or e-posting the file to a contractor. For occasional use this can be a lot cheaper than buying a printer and its ink or toner.

….

Oooh, not in brain-bashing mode at the moment. Bad cough and cold. I won’t even venture down the garden to the cold workshop in this state, though I might manage to fill the bird feeder…

[Nigel Graham 2]

On Nigel Graham 2 Said:

Michael –

Yes, I know CAD does work to as many places of decimals as the computer can spare, and expects lines to meet properly.

[…]

I’ve not tried similar in Alibre, which will say the sketch is not closed; “Open Loop” error I think.)

[…]

Get well soon, Nigel

… and do please try it in Alibre

MichaelG.

.

Edit: __ Whilst you are not feeling well-enough to do anything constructive … Now might be a good time to watch, and listen-to, that tutorial video.

[Nigel Graham 2Participant @nigelgraham2]

Well, I snuffled and sniffled my way through this like an asthmatic hedgehog chasing an athletic snail…

No, as far as I could find you can’t use line thickness in a 3D sense in Alibre but instead we have “Shell”, I was informed a little while ago. So I experimented and discovered a very useful but unexpected effect. I thought it would act like an through-extrusion, leaving rectangular-ish tube, but unless I missed something and stumbled on the correct choice by default, it will leave a box floor in place.

This is the off-side bunker for my wagon, the real thing long ago fabricated from 16swg steel sheet. I thought to draw the doorway sill very slightly high so the extrusion didn’t make a big ‘ole in the floor. In reality it is cut through the edge, and the vertical web of the internal angle joining wall to floor is cut away to create a shallow, chamfered threshold across the opening. I have omitted small details such as the angle-steel frame parts and a stiffening border to the door. (To bring the angle round that front curve, I cut a segment from a turned ring.)

 

That spare plane was to mirror the thing to create its twin but this raised two questions:

1) Shouldn’t it reflect the Shell cavity as well as the outer wall? It was happy to reflect the Extrusion but as a “solid” block, and didn’t want to accept the Shell into the details form.

2) If I mirror an object to reverse its orientation, or to create separate but handed Parts like these, can I delete the original? Or separate them from the single model to place just one, but either, of the two in an assembly? (I tried this with those chassis rail parts but the answer seemed to be “no” to both questions>)

…

I agree I could spend the time watching the rest of that video but I’d not be able to concentrate. This took me quite a while with a lot of tissue-hunting expeditions. Now, where’s that snail gone?

[JasonBModerator @jasonb]

Probably be more successful if you mirror the sketch so you have the 2D of both bunkers. Extrude that sketch. Then when you go to shell click the top of each bunker.

An easy way to just get one half is to sketch a rectangle around the side you don’t want. Then cut extrude through all which will effectively hide that half. You can then “save as” bunker left. Then go back and edit the rectangle and just drag it over the other bunker, deactivate sketch, generate to last and then “save as” right bunker. This is what I do for pattern halves.

 

[David JuppParticipant @davidjupp51506]

Nigel – If you’ve modelled half of the part as a solid, mirror that BEFORE using the Shell tool.  Apply Shell to the solid of the combined original and mirrored features.

The order of applying features is important and will change the final result.

When mirroring there are 2 different tools you can use – which will give different results.

Mirror – is used to select individual features to mirror and will leave the originals also in place.  Take care, it is the action of the tool that is mirrored, which may not always be exactly the same as mirroring the resulting solid.   (NOTE – in version 28, some extra options are added to this tool to give more versatility).

Scale/Mirror Part – this makes an ‘other handed’ copy of the entire part.  It does NOT leave the originals in place.

 

[EDIT – unlike Jason, I don’t recommend using Sketch mirror – I prefer mirroring features, because there is less in the sketch to edit if you have to tweak things later.  Jason isn’t wrong – we just have different preferred ways of working.]

[David JuppParticipant @davidjupp51506]

Oh – and Nigel, higher versions of Alibre do offer ‘Thin Wall’ features which work rather like the use of line thickness that you mentioned.

In Atom3D, you can use sketch offset to automate some of the work if you wanted to do an equivalent.

[Nigel Graham 2Participant @nigelgraham2]

I saved a copy of the file under a different name so I didn’t lose the original.

It won’t let me mirror the original sketch even after deleting everything else. Two actually: the main box and the one for the door.

If I mirror the extrusion the reflection is a “solid” and the shell tool won’t work on it.

[David JuppParticipant @davidjupp51506]

Nigel,  I’m struggling to follow your description – please send file including errors/problems.  Shell is a “special” case, it acts on the entire part – which can get confusing.

[JasonBModerator @jasonb]

If you have deleted everying except the sketch then you can only us ethe mirror that comes up in 2D sketching not the feature mirror that David mentioned above.

So you either need to activate 2D sketch and then you can mirror the sketch, then extrude.

Or you need to do the extrude of the first sketch and then the feature mirror that David suggested will mirror the feature (extrusion) rather than the sketch

Finally use shell and click the tops of both solid bunkers

[Nigel Graham 2Participant @nigelgraham2]

Oo-er- thought my PC had collollopsed again. It went all black and lifeless, but I think it was just the external PSU’s mains plug coming loose. I’m not sure if my later attempt with a copy of the original file has survived…..

Yes, it has but without my attempts to modify it, so let’s try again. This is a very confusing tool indeed!(It’d be a help if I could see both this and the Alibre window easily without forever having to switch off BT’s idiotic home page.)

Right: model mode – only the one Mirror tool (for single, linear copying).

Sketch mode: same. I can pick up Sketch 1 for the basic box and it shows with all its dimensions and construction lines.

 

I can’t do anything with them though. Ah, found the right tool one, or at least one that worked, hiding further along the tool-bar. Managed it, somehow, without really being sure how, then saved it before it escapes or the PC goes off again.

I didn’t try to copy the door from one to the other. I constructed both from new in a single network of lines. The image below is directly after finishing those.

I can never predict which way up anything will be, or align a set of Parts consistently, which is probably the main reason I cannot build up Assemblies. It looks as if the XY plane is really that of the screen at the start, but by the end the orientations of the planes and the model are more M.C. Escher than reality. I have now tilted the model with the very lively View Cube so the XY plane is fairly flat, and though that looks right the Cube says the top is actually the front, and the two bunker sides facing the kerbs are the top and bottom. Good thing I’m not an architect – the wallpaper would be on the ceiling and the water would emerge from the taps, horizontally!

[David JuppParticipant @davidjupp51506]

Nigel,

If you want to edit an existing sketch, right click on its name in the Design Explorer and select Edit.  That takes you back into the sketch, and makes the sketch tools available.  Then you can adjust dimensions, add constraints, use sketch mirror etc.

Objects will be the ‘way up’ that you place them.  If it matters to you, then consider carefully which plane to start any sketch on.

Personally, I don’t worry much about the orientation of parts.  They can be re-oriented when producing 2D drawings or in assemblies.

[JasonBModerator @jasonb]

Save this image somewhere and look at it when you start modeling a new part.

For those bunkets your first sketch was looking down in plan at the top of the bunker so the top on the cube is the ZX plane so pick that to start your sketch on.

If you wanted to draw say the axle you might start with a circle as seen from the right hand side so choose YZ which is th eside of the cube.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou Jason, David.

Going to call it a night – my cold is worsening and making concentration even harder.

[David JuppParticipant @davidjupp51506]

Nigel,  if Jason or I send you a file, you can do the following;-

• Play back the original modelling by dragging the blue ‘dog bone’ up the Design Explorer as far as it will go (below the first feature) – then drag it down one feature at a time, and watch the design develop.
• Right click on any feature or its associated sketch in Design Explorer and choose Edit.  You can then details and make adjustments.

Take care, as it is also possible to change the order of features by dragging them up and down the list. As features built on what was done previously, changing the order can break features.

[Nigel Graham 2Participant @nigelgraham2]

Oh, I thought I’d replied. Must have forgotten to push the blue button.

Thankyou – will do when I’m a bit more in the land of the living.

 

I had another go at trying to understand that Sweep tool, from the Alibre site’s manual. By creating a few straight and curved rods I gain a vague idea of how to use the tool but not how to make the profile run along the guide-line. They traced the intended shapes but in their own parallel world.

[David JuppParticipant @davidjupp51506]

Nigel

In Sweep, the location of the profile sketch ( or sketch to sweep ) fixes the location of the final 3D feature.

The Path sketch only controls the shape and size of the 3D feature, not the location.

It usually makes sense to arrange that the Path and Profile sketches coincide, but the software doesn’t require that.

[Nigel Graham 2Participant @nigelgraham2]

I feel guilty. You shouldn’t be talking shop on a Sunday evening!

I thought I was doing what the instructions said, too.

At least I’m never likely to need the Sweep tool very often, so being unable to use it would not matter much. I’d have to find work rounds, however inelegant, that give near enough the wanted results.

I can’t create assemblies either. That’s more serious but there is a way around that, based on that frame above. It means extra work and is not the “right” way to use 3D CAD, but it might just work if all else fails.

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