Dimensioning Puzzle (Alibre Drawing)

[Nigel Graham 2Participant @nigelgraham2]

I found the fraction / decimal option and tried re-drawing this thing – about the hardest I’ve tried in Alibre.

I had to re-start it completely at least once, and had to make innumerable re-calculations, deletions and corrections, different attempts at single details, etc.

Whether the ends are meant to be parallel with the slot ends or radial would not matter in practice but drawing either form, to the specified thickness, was extremely difficult.

I plotted the axis of the suspension pin then located that straight back edge 0.500″ from there.

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Eventually I had a 2D outline of the basic plate. I did not bother about rounded corners or those weeny holes of unknown size in the corners of the slot. Turning it into a 3D model meant several iterations to find and delete odd scraps of trimmed lines, and careful study of the drawing sheet to find the thickness, which is camouflaged by being on the drawing of the die-block.

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Finally I tried to put those three rivet holes in it. I wanted to work these out myself, but where do I start?

Harris’ drawing omits to tell us, and I could not work them out. So I re-plotted the pin centre and put a circle on it, so I could plot that little step in the bracket to create a bounding rectangle for the rivets to live in by what looked about right.

It struck me that having to draw each of the bracket and the plate as separate Parts risks them not fitting together thanks to dimension errors in drawing their shared details, twice.

Only the pin was now visibly in the wrong place and I have no idea what I did wrong where.

Oh for Heaven’s sake! Start yet again…..

…… I closed the thing down instead.

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It had taken me well over an hour to produce a faulty version of what anyone else would probably knock off all-correct in ten minutes.

[JasonBModerator @jasonb]

Top & Bottom

If you draw the slot and it’s two radial ends first then it should be fairly simple to place the end 5/32″ away. Just draw a random line a bit above the to end of the slot. Then use the constraints to first set it parallel to the line that forms the end of the slot. Then dimension the two lines to be 5/32″ apart. You can then trim away any excess at the ends of the line before finally mirroring it about the ctr line so you have one at the bottom too.

Three rivit holes

Picture shows how I worked out their spacing. Take the 5/32″ notch away from the 1/2″. Take the 9/64″away from that result and then divide that answer by 2 to get equal material either side of the group of 3. Harris may not put it on a plate and give that exact dimension but with a bit of common sense there is enough info to work it out.

Same maths can be done in your head if you start with 32/64 – 10/64 = 22/64.  Then 22/64-9/64 = 13/63. Then 13/64 divided by 2 = 13/128 or 0.10156

[David JuppParticipant @davidjupp51506]

Because so much of the part relates to the centre line of that slot, I’d be tempted to produce an initial sketch which has perhaps just that, as a reference (dashed / construction) arc.  I would then close that sketch.

You can ‘project to sketch’ this existing sketch into any new sketch within the part , and if you select ‘maintain association to source’ the copy will update if you alter the original.   This allows you to easily re-use the centre line arc in as many new sketches as you need to.  You could extend this idea to also include other key construction lines in a ‘master sketch’.

There are many different ways to produce the needed profile.  In addition to Jason’s comments you could also

• set end line of slot perpendicular to the reference arc centre line.
• use ‘offset’ from the centreline arc to produce curved edges of slot.

I’d also suggest – don’t do corner rounds inside sketches, instead use the Fillet tool.  This leaves your sketches easier to edit if you need to go back and make changes, it’s also much easier to ‘try’ different fillet sizes to see what ‘looks right’, if the size is not specified.

Generally keep sketches simple – it isn’t necessary to put the entire profile into a single sketch (in fact that’s often far more difficult).  Four or five very simple sketch/feature pairs is preferred to a single complex sketch with single feature.  If you do make a mistake, simple sketches are much easier to repair, and of less consequence if you do decide to delete a sketch and start again.

Responsiveness of the software will also be better if sketches are simple.

Think of these as guidance rather than rules, you will come across exceptions.

[Nigel Graham 2]

On Nigel Graham 2 Said:

 

It struck me that having to draw each of the bracket and the plate as separate Parts risks them not fitting together thanks to dimension errors in drawing their shared details, twice.

Nigel – to avoid that problem you can ‘copy/paste’ sketch between parts as Jason has mentioned.  You can also make ‘part 2’ within an assembly that includes ‘part 1’ – you can then ‘project to sketch’ aspects of ‘part 1’ into a sketch for ‘part 2’.  You can also manually constrain individual sketch figures to geometry of the other part.

Rather like ‘virtual spotting through’ – but without risk of part slippage.

Basically you don’t need to sketch the detail twice – do it once and then re-use it, by whatever method you are most comfortable with.  You can of course also ‘trial fit’ in an assembly workspace.

[JasonBModerator @jasonb]

As David says the first part of constructing that link that I did was place a ref circle to represent the ctr line of the slot and that also gives the springing point of all the other radii and the radial edges even if it is outside the part (Sorry Martin)

I do usually add holes as a separtate sketch particularly as Pro has some different ways of dealing with holes but put them all on the one sketch to save having to post multiple screen shots. Fillets are separate at the end.

 

This is how I started my sketch for the block, I picked up the three rivit holes and the back edge of the link and copied them. Opened up a new part and pasted them onto the sketch plane. Not only are they already positioned but I still have that springing point as the intersection of my axis.

From there I added the pin hole, one of the lines at 7/32 and mirrored that to get the edges, 3/8″ circle to then have tangental lines added before trimming leaving the 3/16″ radius end.

Sketch then extruded 3/16 about mid plane. Then select another plane and draw a rectangle for the notch snaped to ctr line an ddimensioned 5/32 from pin (other lengths not critical) and cut extrude that to form teh notch

Lastly chamfer inner edge of pin hole for peining over the pin’s spigot.

[Nigel Graham 2Participant @nigelgraham2]

I had made several attempts starting with concentric circles but kept getting them wrong. I realised they want diameters and I was miscalculating them from the radii. So tried using the Arc tool, which at least meant I could use the given radii directly and reduced the amount of arithmetic to go wrong. Though it still did.

The corners of the slot are little holes not fillets, and I did not even try to put them on my last attempt.

The ends of the slot are radial and I managed to draw them, but when I tried to draw the outline ends parallel to them it kept telling me something about “over-constrained” and nothing I tried worked.

Drawing the ends radially was not much better – in both cases I found it very hard to place them at the right distance. The dimension tool appeared to show angles all the time and I’ve no idea what I was doing wrong.

Putting those rivet-holes needed the outline and the pivot pin in the right places to measure from, but I’d somehow messed that up too.

 

Objects like that link seem just too difficult for me to draw in CAD, and I can use the system only for very simple, single Parts I have either designed myself or have re-drawn from much simpler, better-dimensioned drawings.

[David JuppParticipant @davidjupp51506]

Nigel,

Try holding down Shift key when dimensioning circles – that should switch you from diametrical to radial dimensioning.   If you can’t get that to work due to your part properties, just stick with diametrical, but type in 2 * Radius for the value.   If you’ll always want to work with radii, you can change the default behaviour.  Arcs will use radial dimensioning by default.

Holes at corner of slots – do those as a separate feature, not in same sketch as the slot.  Use intersection constraint to fix the hole circles to the corners of the slot (there are other ways).

For ends of link – if Jason’s suggestion doesn’t work for you, try using Offset from slot ends to get started, then ‘extend’ the line to meet arcs and trim to complete.  That aspect is probably the most difficult because of having to work from the slot outwards.

[Nigel Graham 2]

On Nigel Graham 2 Said:

[…]

The ends of the slot are radial and I managed to draw them, but when I tried to draw the outline ends parallel to them it kept telling me something about “over-constrained” and nothing I tried worked.

Drawing the ends radially was not much better – in both cases I found it very hard to place them at the right distance. […]

Just as a small aside: I have [to satisfy my own curiosity] been ‘constructing’ that plate in 2D from the given dimensions, and noticed that the 5/32” dimension is not adequately defined … it matters ‘not a jot’ in reality but this may be sufficient to upset Alibre … is the 5/32” a linear offset, or the arc-length ?

[technically, it cannot be both!]

MichaelG.

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[JasonBModerator @jasonb]

I actually placed the slot ends and the 5/32″ thickness by adding a couple of Nodes on the slot ctr line and the appropriate distance along it. The radial lines can then be drawn from datum to node and then extended out to the required arc. Many ways to skin a cat, you just have to get to know the cat.

[David JuppParticipant @davidjupp51506]

Michael,  the 5/32″ will be a linear offset.  Mainly because there isn’t a dimension option to directly set an arc length.

It is possible to set an arc length (though not obvious) by using some basic maths in the inbuilt equation editor.

[Michael GilliganParticipant @michaelgilligan61133]

Jason/David

I am comfortable that the cat can be skinned … I was merely pointing-out that the original drawing is not adequately defined, and may have been the source of Nigel’s frustration.

MichaelG.

[ should have learned by now to keep my nose out ]

[JasonBModerator @jasonb]

It is hard to tell if the shorter arrow next to the 5/32″ dimension is straight which would indicate an offset or if it is a curve which is more likely to represent an ARC length. My dimension is a straight line between the two points.

For those with a curious mind the arc length between my two nodes which are spaced at 0.15625″ is 0.157328″ a difference of 0.001078″ I’d be happy if I could file to that given the thickness of a scribed line.

What we don’t have is access to any text that may have included additional information

[David JuppParticipant @davidjupp51506]

I’ve now produced models of the part using two differing approaches.  Both worked, but one was much faster (for me – others may have different experiences).

First approach was very much to produce the original as per the drawing – that needed a lot of construction geometry, and quite a bit of thought at times.

Second approach was to model an arbitrary piece of plate, cut the curved slot, and slowly add cuts for holes and to shape the part.  Though I didn’t follow the sequence of operations likely to be used to manufacture the part, I wasn’t too far away from that.   I found this much more intuitive, and I had much less construction geometry in each sketch, as I could refer to edges of previous steps.

I’m not saying either approach is ‘right’ – just highlighting that there are alternatives.

[JasonB]

On JasonB Said:

[…]

For those with a curious mind the arc length between my two nodes which are spaced at 0.15625″ is 0.157328″ a difference of 0.001078″ I’d be happy if I could file to that given the thickness of a scribed line.
[…]

Yes, that was the underlying point of my post

Such differences are trivial in the the real world … but they can sometimes do a very good job of upsetting a CAD package; which might protest either that there is no intersection, or otherwise that a specific line cannot both run in a particular direction and also have its endpoints at specific locations.

… I thought this might be the key to the problem that Nigel reported.

… The ends of the slot are radial and I managed to draw them, but when I tried to draw the outline ends parallel to them it kept telling me something about “over-constrained” and nothing I tried worked. …

MichaelG.

 

[David JuppParticipant @davidjupp51506]

‘over constrained’ is one of the most common messages that Alibre will return – it suggests that constraints/dimensions have been applied which are more than the minimum necessary (mathematically) to fix some aspect of the design.

In the ‘real world’ we often over constrain with no consequence – but in the mathematically perfect world of CAD that can lead to an error.

An example – a rectangular picture frame, in real life we glue and pin at all four corners – but with infinitely stiff rails to make the frame from and perfect joints, we only need to fix 3 corners of the frame – fixing at the fourth corner is redundant.

This does take a while to ‘get your head around’ – there are strategies that can resolve this, but it isn’t obvious.  Usually a less restrictive alternate constraint is available that won’t lead to an error.

[Nigel Graham 2]

On Nigel Graham 2 Said:

 

The ends of the slot are radial and I managed to draw them, but when I tried to draw the outline ends parallel to them it kept telling me something about “over-constrained” and nothing I tried worked.

 

Without seeing Nigel’s file it is hard to be sure but the message may have come up for several reasons.

– Michael’s comment about being parallel and also having the end point located at say the central datum point would be one of them.

-Another may be that it was already parallel and the CAD did not like being told twice

-One end of the line may have snapped to another feature that Nigel did not notice and that was preventing it from being made parallel to the end of the slot.

-clicking the unconstrained line before the constrained end may also make the message come up as the convention is to constrain the second item clicked to the first.

-probably a few other reasons too.

[Nigel Graham 2Participant @nigelgraham2]

It certainly wasn’t at all obvious. I couldn’t make it work even by just drawing a short line not joined to anything.

It does not matter from a purely mechanical point of view, so if it needs a rotary-table to make much of the rest, the ends can be radial too.

They’d hardly be noticeable. What matters more is why I could not make a particular CAD move work, rather than what it is for, since some other application might need lines to be parallel.

 

I take it that the order does matter then. In many of my attempts the wrong line would move.

””””’

To regain some sanity I copied a far simpler drawing, part of the Stent T&C Grinder. The peculiar thing here was that it was drawn upside-down originally, making the two countersinks (I changed them to counterbores) hidden details. I had think hard which way round it goes, to draw it the right way up, helped by the part-assembled project standing next to the computer. It was of course also chain-dimensioned, and in vulgar fractions.

 

[David JuppParticipant @davidjupp51506]

Yes – selection order does matter for applying sketch constraints.

If neither line is fully fixed, the second one selected will move to be parallel with the first one selected.

If one line is fully fixed, it will be the other one that moves.

So the first selected figure becomes the ‘driving’ one, unless pre-existing constraints or dimensions prevent it.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou – that’s often caught me out!

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