Dimensioning Puzzle (Alibre Drawing)

[Nigel Graham 2Participant @nigelgraham2]

Err, I think I’ve backed myself into a corner.

I don’t know how readable the attached drawing will be on here.

I’m adapting the K.N. Harris version of the motion-work for LBSC’s ‘Maid of Kent’ design, for my steam-wagon’s engine: the cylinder sizes are similar enough.

I’ve drawn the Expansion Link in decimal and angular format so to make all the arcs and holes by polar co-ordinates and rotary-table; but cannot see how to dimension the straight back edge of from the link centre-lines, hence derive its distance from the origin. I can work it out and describe it by a Note, but I want to be able to verify the dimensions within the drawing itself.

For this edge, according to Mr. Harris, potentially controls the suspension-point’s location, although he does give the important distance of that from the slot centre.

The arcs all obligingly provided their radii, so if pick the intersection of any one of them with the horizontal line – which I cannot see how to produce in either direction on the Drawing – it simply repeats that.

 

Nor can I see how to enter centre-lines between non-parallel entities the ends of the slot (the overall length is easy, from the side elevation).

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Only, I’ve turned a rather confusing original drawing full of thirty-tooths (and I found an arithmetic mistake among them!) into a complete puzzle. Alibre can tell me exactly what I had drawn, but I can’t see how to ask it the critical one.

I can calculate the polar co-ordinates to drill those three small holes as I have placed them, but I would like to use the system’s own maths to confirm my placing w.r.t. the centre of the link. The original drawing dimensions this assembly in a rather back-and-forth way.

A thought: would it work if I put all the lines on one Layer? Or would that create other difficulties?

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[Whether I will ever build the locomotive as well, from the part-made chassis and set of castings I bought some years ago, is another matter! Project Number One is the steam-lorry but it makes sense to batch-make common parts, even across projects.]

Now what have I done? The drawing’s fallen off. So apologies if it appears twice…

 

 

 

 

 

 

 

 

[Michael GilliganParticipant @michaelgilligan61133]

I cannot advise regarding Alibre … and would not presume to try … But I will give you the small encouragement that one instance of your drawing is visible in the post.

Visible, but not very easily legible [but that’s presumably a forum problem]

MichaelG.

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Edit: __ This screenshot of a pinch-zoomed area should nicely illustrate the disappointing quality of presentation on the forum page:

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[JasonBModerator @jasonb]

First dimension the radius or diameter of one of the arcs that make up the curved slot, place dimension on the inside of the arc not outside That will establish a ctr point on the drawing sheet this comes up as an orange dot which being the ctr of your rotary table is the ideal datum to then work from.

I have then used that point and the various small circles to dimension their ctr position from datum

I have also dimensioned the flat edge from the datum.

PS I would not presume the quality of the captured alibre drawing is a forum problem. You get out what you put in.

[Martin ConnellyParticipant @martinconnelly55370]

What snap points are available for you to dimension from? Can you select the centre point of a line, straight or curved?

Martin C

[JasonBModerator @jasonb]

There is another way. As you will have entered dimensions when creating the part file you can have these dimensions brought forward onto the 2D drawing but I seldom use that option as it can get messy.

When starting the 2D drawing the window that comes up with the various views in pastel colours has a big box “more options” if you click that at the top of the list is “design dimensions” if you tick that all your sizes used to create the initial part will appear on the 2D drawing. However they are placed as you did when construction the part so are likely to need dragging about to more suitable positions unless you are very particular about their initial placement.

[David JuppParticipant @davidjupp51506]

Nigel,

Something like this?  Not sure I’ve grasped what you are actually wanting…

The ‘trick’ is in order of selection – the ‘slot’ dimensioning tool only appears if (with dimension tool active) you select a straight edge and then a circle/arc.  A dialogue should pop up offering a number of choices about how the dimension is to be arranged – you may have to try more than one to get what you need.

You can use the same ‘slot tool’ to dimension your small corner holes relative to the straight edges of your part (or to any straight line that you add to the view).

[JasonBModerator @jasonb]

David, how are you getting the dotted ctr line to show down the middle of the slot? When I place my sketch elevations I don’t get that even ticking show ctr lines. This means I can only dimension from the straight edge to one of the sides of the slot not the ctr line

It would be better to dimension the vertical edge back to the datum wher the cts of the radii are then all sizes can be taken from that datum eg zero DRO on ctr of rotary table.

[David JuppParticipant @davidjupp51506]

Jason,

I used the centre-line tool to place the centre-line

https://help.alibre.com/articles/#!alibre-help-v27/2d-drawings-detailing-annotations-and-gdt-annotations-centerline

I admit I struggled to make sense of Nigel’s posting – I may well have misunderstood what he wants to achieve.  The Alibre slot dimension tool can be useful for any edge/line to hole/arc dimensioning need.

[JasonBModerator @jasonb]

Thanks David, simple once you know it’s there, another one to remember for future use.

I get the slot options come up Ok and do somtimes alter the option number but most of the time Alibre seems to pick the one you want anyway.

I think it is the right of the two red dimensions shown here that Nigel wants but could be the one on the left. I was going to draw his part exactly but without one of those it can’t be done. position of the 3/16″ holes also missing.

[Nick WheelerParticipant @nickwheeler]

The lack of any dimensions for the straight edge was the problem for me as it, and the hole layout, depend on each other but aren’t positioned in relation to any of the other  features. As it’s symmetrical only half needs to be drawn which usefully simplifies the basic sketch.

Like everyone else, defining everything from the centre of the radii is what I would expect. The whole thing looks like it’s meant to be marked out and mostly made by hand after drilling the holes – the four holes at the ends of the slot wouldn’t be necessary if it was milled using a rotary table for example. But once a CAD file is available, it looks like a perfect candidate for laser cutting….

[JasonBModerator @jasonb]

Just bolt a bit of plate to the rotary table. Add a couple of angles for the chamfered corners and it can all be done at one setting. The holes in the corners or a larger half round at the end were often use dso the die block could run out into the gap and not leave a ridge as the link wears.

One I made earlier, I’d bang it out on the CNC now.

[David JuppParticipant @davidjupp51506]

Like so (obviously my sizes are random – just to show that the dimensions can be placed).

[Nigel Graham 2Participant @nigelgraham2]

Dave –

Ah – that is what I want, but I could not see how to do that. Each time I selected the centre-line it obligingly quoted the radius. I could not select that centre-point

This link differs from Jason’s, which seems to be for a traction-engine with its suspension-point beyond the end of the slot. Mine is a locomotive type, with central suspension offset behind the slot slightly.

The three small holes are for rivets that hold the two lifting-link brackets on, and the original drawings give you some rather awkward arithmetic to place everything as they should be.

 

The lifting-link trunnions are on the horizontal centre-line a set distance back from the slot centre-line. The assembly in in three separate parts, and as the original drawing is not easy to work out I decided the CAD could verify my sums, but could not see how arrange that!

The two 3/16″ holes’ locations are measured on a radius from the same centre as the rest. (The crankshaft axis on the finished engine.) That radius and the height above and below the centre-line are on the K.N. Harris drawings, but I could not see how to put the radius on the Alibre drawing. Their heights are on the side elevation, along with their angles, to set them out by polar co-ordinates; but that still needs the radius on the drawing! I think I’d have to do that by a note.

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The original drawings probably date from when many constructors had to use manual marking-out methods, saws and files for tasks like this, and did not envisage alternatives like milling-machines with rotary-tables. And DRO units: my example has radius and p.c.d. functions but I’ve not tried using them. However I am used to its normal Cartesian co-ordinates and combining those with a centred rotary-table to work to polar co-ordinates seems logical for making largely arcuate components. That could include features not obviously on an arc, like those rivet-holes.

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Jason –

“Just bang it out on the CNC”… indeed. We don’t all have such sophisticated equipment!

Yes – I was envisaging making these links on a rotary table as you show. Only being loco links they are more complicated than your TE pattern one, with fiddly lifting-link trunnions.

Although my links are for a steam-wagon the engine is an enclosed vertical unit, not an overtype, so the motion has to be compact to fit in the box. I chose eventually, adapting Harris’ version of the ‘Maid of Kent’ link-motion is probably as good a way as any. The original engine was a compound but with only 90psi working-pressure and no superheater, a simple may be better and the two cylinders are near the size of the locomotive’s.

I know the dimension-import tool you mean: it can certainly produce a tangle of arrows and numbers! I used it then edited the results, as shown by the “in 4 places” and similar notes.

You are right: it would be the right-hand one of your two red dimensions I want.

I had calculated the locations of the 3/16″ holes but not shown their radius from the centre because I could not see how to… apart from as a text note. I planned that they need only the radius and angle to describe them. The angle is quoted on the side elevation.

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Nick –

The original design is referred to the crankshaft centre then the slot CL, in that order, but the straight back has to be derived from a rather roundabout collection of fractional dimensions on the separate parts to be rivetted on.

Very likely LBSC then K.N.Harris assumed cutting the slot by hand but that is not the reason for those squared-off ends – which would give more work in their production. (In full-size manufacturing they were sometimes made on a slotter with a power-driven rotary table; giving square ends.) The die-block matches them and makes the assembly more compact than if the slot had semicircular ends. The little corner holes assist making but more importantly give slight overlaps for the die-block in full gear.

I had said nothing about contracting their cutting; but I was asking about how to dimension the drawing, not how to make the thing.

Yes, I could have drawn only half and mirrored it, but it would not have made much difference.

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Martin –

Locating the centre-point of a line or arc…. In the 2D Sketch, probably; but is it possible in a Drawing?

Selecting any arc just told me its radius every time.

[JasonBModerator @jasonb]

You have two options for dimensioning the 3/16″ holes, assuming you were able to place them correctly when modelling the part using angle and height.

1. You can dimension them in x and y and then just use the x and y axis of the mill to position them. No backlash problems if you have a DRO. it does need that central point to do it though.

2. You can do as the original drawing and dimension as angle and distance then rotate the table but getting the angle onto the drawing is not so easy and you also have backlash of the rotary table to think about. Though you have managed to get the angle but that was by adding as a note so no double check on the actual geometry.

But I will say you have done well to model the part in the first place and get what you have on the 2D drawing.

Might want to think about increasing the height of the text as I find the default 9pt a bit small, it will make it easier to read in the workshop and also clearer if you post any more images here, try 12 or 14pt Ariel. To do that click “dimension styles” at the top of the screen. On the screen that opens select “text” down the left hand side, you can then click the box with “A” in it and that brings up a window with font size and style, choose what you want and before saying OK tick the “make default” box then you won’t have to do it again.

[David JuppParticipant @davidjupp51506]

Nigel,

As Jason showed in his first response, dimensioning an arc (even if you ultimately don’t want that dimension) will add a yellow/orange node at the centre point – you can use that to add further dimensions from.

The ‘slot dimension tool’ I mentioned gives another way to tackle this.

If desired you can add items (e.g. points and ‘construction’ lines) into a drawing view manually if that will help to generate your desired result (right click within the bounding box of the view, choose Activate Sketch in View).  These can help with subsequently adding angles…

I have only the most basic grasp of steam engine valve gear – so most of your description means nothing to me.  Given a simple enough description of the desired outcome, I can advise how to achieve it in Alibre.

[David JuppParticipant @davidjupp51506]

Jason (& Nigel) – things like font size are inherited from the drawing template.  The ‘set current settings as default’ will only apply to drawings on blank sheets (no template used).

It is possible to edit the provided templates – though these are set ‘read only’ in Windows by default.  Probably better to open the template file and ‘Save As’ to your own location, and then adjust the properties, add logo, etc.

Nigel – Atom3D has reduced abilities regarding template editing (can’t add new fields or labels).

[Nick Wheeler]

On Nick Wheeler Said:

As it’s symmetrical only half needs to be drawn which usefully simplifies the basic sketch.

 

True – but one real beauty of 3D CAD is that effort savers like that are done in the 3D part modelling.  Then the 2D drawing (of the complete item) drops out almost for free.

In my most recent example above I modelled only one of the 3/16″ holes, then mirrored it (in the part) – the drawing automatically shows everything (unless I deliberately hide something).

[JasonBModerator @jasonb]

I did it the same just mirroring the holes when modelling the part and use that a lot together with extruding equally either side of the plane that a sketch was done on.

I don’t tend to use the supplied templates, for my own use a plain sheet is good enough. For a set of drawings that will be published I will create the first sheet with title etc from a blank and use that as the template for subsequent sheets so my default settings do get carried over.

Activate sketch in view does allo a “Node” to be added to the 2D drawing once the initial centre point has been established which is better than having the arrows point at nothing.

You can also make use of it by adding another elevation and drawing circles to represent cutter diameter then set them tangent to the various surfaces. You can then dimension the offsets that you need, probably more useful when using imperial cutters for example doing Nigels 7/32″ slot with a 1/4″ cutter running down the middle then a finish pass along each edge.

[Nigel Graham 2]

On Nigel Graham 2 Said:

“Just bang it out on the CNC”… indeed. We don’t all have such sophisticated equipment!

That’s what I did when making an expansion link set for a fellow traction engine builder:

In the CAM program I left the slot undersize by 0.01mm and the mating die block was CNC machined 0.025mm oversize. The slot was finished by draw filing using Hoffmann roller as a gauge. Finally the die block was filed to fit the slot. Material was 1/2″ thick gauge plate.

I’ve learnt about the Alibre centreline command from this thread.

Andrew

[Martin ConnellyParticipant @martinconnelly55370]

Nick, when I worked as a manufacturing engineer I had to check drawings before they were issued for use in production. Any that had a datum where there was no material were rejected straight away. If you could not inspect it easily after manufacture then it was designed in cost. If you had to work out dimensions from a point in space it was error prone and time consuming so once again designed in cost. For complex parts I often redrew them in CAD because if I could not it showed up missing dimensions on the drawing.

Martin C

[Nigel Graham 2Participant @nigelgraham2]

Martin –

I understand your industrial practice but model-engineering drawings were never as demanding, and I am trying to translate one that breaks all your professional rules into ones I can use with my tools (errr…. and ability!). I want the parts right but my drawings don’t need follow trade formalities.

However, you do make the point that CAD can find missing dimensions – that’s more or less what I was trying to do but had somehow got lost on the way.

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Jason, David –

I am trying to verify my own version of an old drawing that is dimensioned from a centre not shown on the paper, and also has vulgar-fraction dimensions that sort of loop back on themselves.

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To make it more fun, the drawings cover two versions. That link is on both sets but although those 3/16″ holes are shown by height and on a circular centre-line on both, the radius is omitted from one of the drawings! In both cases, the back edge is left un-dimensioned, as are the sloping ends, for the builder to work out as best he can.

David – You say you are not clear what these links are for. That’s fine. Just treat them as drawing and making objects. After all, in most contract-engineering workshops you do not know what “Block A43a” or “Pt. No. ZXY5433” even go inside – and usually, are not meant to know. The three little holes hold a pair of brackets, on each side, with trunnions by which the link is suspended in the mechanism, and the trunnions need be a definite distance back from the centre of the slot.

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Aha! I have just opened the drawing in Alibre and wandered around the tool-bars a bit.

I have found the radial centre tool – it is off the “paper” at the scale I used. Plus those other dimension and other formatting menus.

I stripped the two height dimensions from the two small holes, and that revealed an extended centre-line that stops with orange dots just left of the slot centre-line, and just outside the outline to the right. So there is a CL intersection but I can’t dimension from it to anywhere else. The dimension wants to go from the dot instead.

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I found the centre-line tool on the regular Drawing menu and the main tool-bar by exploring, and that obligingly put the centre-line on the slot.

The aspect I find hard is knowing exactly what elevation each coloured tile will produce. They are named but I am not sure what are Left, Right, etc. relatively to my Model image. Is the Preview image in the menu meant to show them? If so, how do you ask it to do that?

I have found the arrows next to that image flips it around but the caption stays as “front view”, and the preview does not reflect switching the coloured elevation buttons.

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Thank you for the formatting tip. I was using the formatting tool-bar on the dimension menu itself, but do sometimes find it difficult to assess how large the characters will be on a print.

I don’t use the supplied templates because they give a lot of space to information necessary commercially, but not for model-engineering in our home workshops. I have tried to create my own, one in inches the other metric, with some limited success.

I did wonder if that drawing would be clear as a .jpg picture on here. I have not yet grasped the formatting subleties, Layers and so on, so the lines tend to all look the same and rather thin.

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The original LBSC / Harris drawings specify “ground stock” for these links, but is that “precision ground mild steel” or “oil-hardening gauge-plate”? Probably the latter, without hardening and tempering it, but do wonder if a mild-steel link with a cast-iron or leaded-gunmetal die-block would be fine. The full-size engines probably used cast-iron for both, or a mild-steel link and cast-iron block.

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The lack of an illustrated centre for all those link arcs may be due to this being, typically, a sheet full of very many components arranged to fit the paper.

You need study the assembly-drawings or any construction series carefully, or understand the machine generally, for the parts drawings do not show positively that all these arcs are concentric about a single point, nor where it is, only their radii.

This, LBSC’s 5″ gauge ‘Maid Of Kent’ design modified by Keith Harris, is not a beginner’s project, but how many tyros as LBSC called them, building much simpler locomotives really struggled thanks to drawings of similar standard?

[JasonBModerator @jasonb]

Gauge plate is the often used material for expansion links.

The arrows flip the preview image about and what you then see will be the central tile, you then pick which other elevations you want. Depending on how you placed the part when doing the 3D model it may not open up with what you consider the “front” in the preview so the arrows allow you to choose your front then the tiles default to the usual plan below and one elevation to the right (subject to 1st or 3rd angle default)

I would suggest forgetting about layers, you don’t really need them for workshop drawings or even model ones to be shared/published

[Nigel Graham 2Participant @nigelgraham2]

Ah – I see. Thankyou. I thought there should be a connection between the preview and the elevation tiles, but I couldn’t see what.

I thought one use for Layers is setting different types of lines, typically fairly thick solid ones for outlines and thin chains for centre-lines.

 

 

I have copies of two CAD primers written for model-engineers, one by D.A.G. Brown, the other much more up-to-date but I can’t cite it because I am not sure where it’s gone! These go into the much further use of layers for separating areas of drawings – I think also used in photo-editing software. Brown illustrates this with the extra two copies of a tender wheel and axle-box sub-assembly you need only draw once in its own layer, but that is in fully orthographic-only drawing. Not like Alibre’s elegant Model-assembly system allowing multiple copies in one click each.

They can be useful in 2D drawing for colour-coding different components, but I found it too easy to make mistakes like putting an entity in the wrong layer, and I realise in Alibre you give each Part its own colour if you need differentiate it in the Assembly.

Anyway Alibre helpfully puts centre-lines in for you (as a layer?).

[David JuppParticipant @davidjupp51506]

Nigel,

Not sure from your latest if you have remaining questions/problems or not.

Layers in Alibre 2D drawings are as you surmise basically for managing line appearance – there are a number of default layers, but you can also add your own. I often add an extra layer with visibility turned off when I want to do more complex things than the standard ‘Hide’ options provide for in the drawing.

‘Weight’ is the thing to adjust for line thickness of a layer – also experiment with the setting of the ‘Realtime Line Widths’ option in System Options -> Drawings -> Viewing/Interaction.  That setting affects the on screen display (printouts should always match your line weight settings).

[Nigel Graham 2Participant @nigelgraham2]

David –

Thankyou.

My query was to try to escape a sort of mental block that arose when I tried to convert a rather mixed original dimension system into one I thought would be more logical for making the part.

The link’s curved front and curved slot are formed using a rotary-table, so I tried to re-draw it in Alibre in a corresponding way. The two 3/16″ holes are also dimensioned on a radius, on the original drawings: and all radii are concentric and centred on the axis of a shaft a long way from the link.

So far so good.

Then I was faced with extra features dimensioned originally in rather roundabout ways,  that add complications of their own. The critical dimension for those is from the centre-lines of the slot to a pin on a bracket rivetted on via those three small holes, not on the link itself as drawn.

Jason’s and Andrew’s photographs show a different, and much simpler, version of the same functional component. Effectively the type I am using replaces that large hole out on the end of theirs, with a pin set off-centre on a bracket in the middle – two brackets actually, one on each face.

I was baffled by trying to dimension from that centre-line intersection to the long straight back edge and the holes, to verify my arithmetic.

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I wondered if drawing the complete assembly would help. It is 5 separate pieces of steel (1 link, sandwiched between 2 brackets with their pins) with some quite critical dimensions involved.

Well, one side of it anyway, an Assembly of just one bracket and the link. That must involve aligning it by at least two features, and I would find that hard enough.

This item is not an easy proposition at all, neither to draw in CAD nor to make physically! Especially without all that CAD/CAM luxury.

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I take Nick’s point that dimensioning anything from a point out in fresh air is bad, but in this case I have no choice.

[Author]

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