Help! Alibre: Changing Part Size?

[Nigel Graham 2Participant @nigelgraham2]

I have searched everywhere on Alibre itself and its own ‘Help’ site…..

How do I change the width of a Part, please, hopefully so the small increase is symmetrical and is reflected in the elevations and Assembly?

Or even, can I, without having totally to re-draw everything I have so laboriously drawn? (Or having to edit the print, manually.)

I need widen one component slightly, without affecting anything else; but all the dimensions in the Part’s own sketch, model and Elevations are “parameters” set in stone… well, cast-iron.

This is also so I can use two of those Parts for somewhat different versions of themselves.

 

”””’

944mBar on the barometer here…… (22:55 GMT)

[Nick HughesParticipant @nickhughes97026]

Could I suggest that you register on the Alibre forum, as it is easy to upload the model file there and thus allow anybody willing and able. to download, see how the component has been designed and then suggest a solution.

An alternative is to open a free Dropbox account, upload it there and post a link here, for the same reason.

Working on the problem file directly is easier than trying to second guess the problem and would probably have helped with a lot of the other problems that you have encountered in previous posts.

Nick

[JasonBModerator @jasonb]

A lot will depend on how you have gone about creating the 3D part and whether the size you want to change was part of a 2D sketch or the size of the extrusion. Then there is the need to keep thing symmetrical which will be easy if the original was sketched with symmetric constraints or extruded from a mid plane or harder if not.

As said above having the file available would make things easy which can be done on the Alibre forum, failing that post some screen shots here.

Funnily enough I was doing similar last night changing two parts that I originally modelled as finished parts and I made a copy which was then altered to be used as a pattern with machining allowances, draft angles, core prints, shrinkage, etc all added and it wa snot too hard to do.

[David JuppParticipant @davidjupp51506]

Nigel – the whole point of 3D CAD is that edits to the 3D model will automatically update the print (2D Drawing).  This is where the biggest time saving comes in.

As Jason mentions, without seeing your file and knowing which direction ‘width’ is in, relative to how the part was originally modelled, it’s difficult to give an exact answer.

It is likely to be as simple as editing either a dimension in a sketch, or the depth value for an extrusion.  Then not forgetting to ‘regenerate to last feature’ to fully update the part.  After that open the corresponding drawing and ‘re-project views’ to update it.

There are other options – such as performing a scale operation in only one direction, but that’s probably best reserved for special cases.

[JasonBModerator @jasonb]

Oh and don’t forget if you want to keep the original part make sure you use “Save As” when saving the modified one otherwise the original will be overwritten.

Parameters are generally only set in stone by you as they are sizes entered at the 2D sketching stage, it is only the “Driven” ones that are hard to change unless the Parameters driving them are changed

[David JuppParticipant @davidjupp51506]

Nigel,

This Alibre training video includes how to edit an existing part – wind through to about 7:45 and watch from there onwards

 

[Nigel Graham 2Participant @nigelgraham2]

Thank you Chaps.

Not sure if this will work, but I’ll try putting the image below….. Oh! It did!

I “made” this cylinder block 3 inches square in section but when I designed the covers (using TurboCAD in 2D mode for the geometrical construction) realised they need be a bit over 3″ dia for the geometry to work, and to avoid the nuts overhanging the rims.

So I need increase the block’s width; only by 1/8″.

I modelled the block from a rectangle and circles, so the dimension to be changed is the width of the originating rectangle before extruding it.

[JasonBModerator @jasonb]

First off I would suggest you click the icon to make sketches show as faint red lines which will make it easier for you and anyone helping to see how you have gone about modeling the part. Atom should have something similar to the one I have ringed in Pro, Probably towards top right.

You could then simply right click on the red rectangle that was used to create the 3″ square and select edit. However if you look down the tree on the left of the page you will find one of the early sketches will be the one you used, again right click and select edit

 

This will bring up the sketch with all the dimensions you entered when constructing it

double click the lower 3″ and then simply type 3.125 into the now highlighted box and hit return or click the green tick

You will then see the line of the sketch has become wider than the grey original part.

Click deactivate sketch top left and then Generate to last top right and you will now have a wider cylinder block.

If you did not originally make the 3″ square symmetrical about the mid plane you can do that just after entering the 3.125″ by either using the symmetrical constraint or adding a dimension from the ctr line to one edge of 3.125/2

[David JuppParticipant @davidjupp51506]

Nigel,

Did you look at the part of the video that I suggested?  It explains exactly how to modify sketch dimensions and extrusion depths.

If you really just have to alter the width of the rectangular profile sketch, just edit the relevant dimension that control the width of the sketch.

[Nigel Graham 2Participant @nigelgraham2]

Oh, I don’t know what’s happened but I had already replied but part of that is missing then yours and Jason’s posts appeared!

Yes, I did study the video, thank you, but I could not make it work properly.

It seemed to keep the cylinders on the centre-line of the expanded block (only 1/8″ wider) but leave the pattern of stud-holes where they were. I don’t know if it similarly put the ports off-centre. I didn’t look.

I could test the centre-line to edge distance by dimensioning but I don’t know how to dimension the locations of small circles like those, in a sketch.

Daft thing is that it’s only the two low-pressure covers that are affected. I’d taken hours to construct their geometry, finding they need be a bit over 3″ dia. then forgot that when I drew the block. I cannot predict what the overhangs will do at the crank end where the block is screwed to the enclosed vertical engine’s case. On top, as in this image, they don’t matter mechanically but look horrible.

I closed the drawing without saving its editing.

 

If the worst comes to the worst I’ll have to redraw it from new, but that takes hours, I think it took at least two for the ports alone. I’d have to add internal details like the passages, manually, on a print, anyway.

[SillyOldDufferModerator @sillyoldduffer]

Never used Alibre, but FreeCAD, Fusion, and Solid Edge can all do this by selecting the side face, sketching a same size rectangle on it, and then extruding the sketch by 1/16″   Repeat for the other side.

As this is a bit clunky, there are better alternatives.  For example, assuming the model was started by sketching the base rectangle, then going back to that sketch in the tree (left panel), and editing the width dimension would do the trick in FreeCAD and Fusion.  I believe Alibre is much the same, as is SolidEdge in Ordered mode.  The dimension is changed in the tree where it was first set.  In effect, you go back through history, make the change, and then the software automatically reapplies later changes to the resulting solid (unless the change breaks something.)

Dead easy when SolidEdge is in Synchronous mode.  There is no history.  Instead just select the face and wait for the extrude arrow to appear.  One of the extrude options tells it to extrude the opposite face at the same time.  SE synchronous is excellent for this but it’s a steep learning curve, so don’t abandon Alibre!  It’s all easy when you know how!  Like learning Serbo-croat…

Dave

[David JuppParticipant @davidjupp51506]

Nigel, you have my e-mail address.  Send the file to me, I’ll produce some images showing how to edit the sketch.

It sounds like your sketch for the bolt holes was dimensioned from a side, but that shouldn’t be difficult to adjust.

Gaining the ‘feeling’ for how to set out parts to make them easier to subsequently edit does take some experience and practice.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou David.

I created it by:

A rectangle across which I drew construction lines for the main centres. Then two circle on their crossings for the cylinders.

Extruded that.

Sketched two reference circles on those centre-lines intersections, placed a circle on the centre-point between the cylinders then used the circular copying tool to generate the pitch-circle copies.

Extruded those to depth on one face, then turned the block over and repeated the exercise for the opposite face.

Then produced the centre-lines on the ends on which to base the ports – a lot of construction-lines involved.

So nothing was made by dimensions from the edges, it was all generated from the centre-lines. The dimensioning from edges was derived in the elevations.

Thankyou for the offer, but I’m a bit confused because I’ve also a message, on here, from Jason.

[Nigel Graham 2Participant @nigelgraham2]

Dave (SOD) –

Oh please don’t muddy the waters by How To Do It in other makes of CAD! 🙂

All that baffling, undefined “ordered” and “synchronous” stuff was one reason I rapidly abandoned SolidEdge. That baffling choice matched why I can’t use TurboCAD in 3D mode: only one right of two or more ways in each case, no explanation which and why, so ruined work.

Alibre Atom is free of such over-complications – though still very hard.

[Nigel Graham 2Participant @nigelgraham2]

David J. –

Thankyou, but sorry, I don’t have your e-post address.

I don’t know if it was on a message in this site’s ancien regime.

[Nigel Graham 2]

On Nigel Graham 2 Said:

 

Thankyou for the offer, but I’m a bit confused because I’ve also a message, on here, from Jason.

We have both offered to do the same.

[David JuppParticipant @davidjupp51506]

Nigel,

You have e-mailed me before (at Mintronics).

If you ever get stuck with Alibre, you can always use Alibre Support

https://www.alibre.com/alibre-customer-support-ticket-entry/

 

[David JuppParticipant @davidjupp51506]

I suspect Nigel panicked when seeing the initial effect of editing the 3″ dimension – so didn’t proceed any further.  If he had done so all would have been well.

Remember that as long as you don’t save the file, you haven’t destroyed what was there before editing.  The images herewith show the process and result.

 

[Nick HughesParticipant @nickhughes97026]

It may be the viewing angle, but it looks as if the cover stud holes are no longer concentric to the bores and so may also need some further investigation.

[David JuppParticipant @davidjupp51506]

Nick – looking more closely you are correct.  The circles for the bolt holes were not fixed in any way at all,  they may have been projected form the cover (which I don’t have).  The PCD size isn’t any obvious fractional inch value.  EDIT ,  ah no, just patterned from the mid line bolt hole.

 

[David JuppParticipant @davidjupp51506]

I fixed things and did some simplification (to my mind) in the process.

I’ll send the file to Nigel.

[David JuppParticipant @davidjupp51506]

There is a simpler way to edit Nigel’s model, by first adding a dimension to the initial sketch and using it to move the block outline up by 1/16″ – then changing the 3″ dimension to 3 1/8″ brings bores back into line and all the later features ‘behave’.

I did the extra things above because there were various items in sketches that were either not fixed in space, or were complex to edit because of the choices made when originally creating them.  The extra changes resulted in a much more robust model.

[Nigel Graham 2Participant @nigelgraham2]

David:

“…. The circles for the bolt holes were not fixed … may have been projected from the cover. The PCD size isn’t any obvious fractional inch value. …. just patterned from the mid line bolt hole. “

No, they were not projected from the covers, though I don’t know how to do that anyway.

The PCDs were not meant to be defined directly, but set by the geometry.

The cylinder bores are 1.25 and 2 by approximate scale from sparse historical information.

The centres are at 2.25 inches as that seemed to approach one-third size of a prototype for which no drawings exist.  The best I have of the engine is an enlarged photocopy of a builders’ publicity photograph over 100 years old, of an unfinished lorry. The inverted-vertical engine’s top covers are very prominent so have to look nearly right; but I also knew the original crankshaft, inside a casing, had a centre main-bearing, ‘cos the advertising said so!

So then I could construct by applied geometry, sets of circles that satisfied all the criteria and put the central stud mid-way between the walls. I had to use TurboCAD in 2D-only mode for that, but it gave me the dimensions from which to draw the covers in Alibre, and produce their derived elevation-drawings.

To base the holes in the block I repeated the same construction, now I knew the cut-line between the plates crosses the centre of the stud, and I knew the outer diameters….

….. Including the LP diameter I had forgotten is over 3 inches.

Which is where it all went wrong.

…….

I now don’t know where I go from here; only that I don’t want to waste a second block of expensive cast-iron.

[David JuppParticipant @davidjupp51506]

Nigel,

From here I’d suggest that you run through the steps of your design with someone who is experienced with Atom3D, and basically repeat it from scratch.

Some very basic changes in your first sketch would have made all the subsequent editing much easier, and eliminated the need for much of your later construction geometry.

Putting central stud hole mid way between the cylinder walls in Atom requires only addition of a single reference line to locate it – but I know that until you’ve seen how that’s done it’s like ‘black magic’.

Once you have that central stud hole, you can simply circular pattern it about each bore axis.

As mentioned – I and others are happy to help BUT, if files exist we need to have access to them to see what you have done.   If not possible to be done in person, screen share is next best, followed by video (which you have repeatedly told us you can’t learn from).

Setting out the logic of the cylinder layout as in you latest post is very helpful (and it was very clear) – that helps us to know what you were trying to achieve.  That kind of information is gold dust.

I’ll produce a version of your block with just block, bores, and top set of stud holes and send that to you – I’ll make an assumption for the sideways location of the pair of bores in the block, but will set it with a dimension that you can change.

 

 

 

[Nigel Graham 2Participant @nigelgraham2]

Thankyou David.

To place the cylinders and stud, I made a horizontal centre-line along the block’s length, three perpendicular ones dimensioned from one end, then put the circles on the intersections. I already knew the spacing. The rest then sprang from those three centre-points.

That was quite easy, but I had no idea the whole drawing was such a mess it gave you and Jason so much work to unravel it. It all seemed to be working, and showed no error messages only their programmers can understand, so I assumed I was using it correctly.

.

The cylinder and valve-spindle centres are already set along with the overall dimensions of the whole engine. I’ve made the crankshaft, eccentrics and eccentric straps, so I have to make the replacement cylinder-block to those.

The problem was setting the covers’ outer diameters and bolt-hole patterns. I solved that as a 2D geometrical puzzle, to give me the dimensions to use in Alibre.

.

(I can’t use Alibre to create individual drawings of the crankshaft and those other components. Even if I could, a 3D CAD Assembly of the 13 parts, complete with the eccentrics’ angles of advance, is probably impossible. One of the entire engine Assembly is certainly impossible, despite preliminary orthogonal elevations to plot everything. Same with almost all of the rest of the project as we’ve shown I can only draw very simple individual Parts and very basic, 2 or 3 part Assemblies – and very badly.)

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