Hopeless…Alibre Ass

[blowlampParticipant @blowlamp]

Nigel.

“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.”

Is there any chance of you posting a rough sketch of this part and I’ll try to show you how it could be done by Direct Modeling?

 

Martin.

[JasonBModerator @jasonb]

He can’t produce reliable parts at the moment so whatever he chooses is going to be a challenge. If he is using one unreliable part to directly produce mating ones then they will both have errors. At least doing separate parts there is a chance of the errors being flagged up when he tries to assemble them.

 

 

 

 

 

 

 

[JasonBModerator @jasonb]

Middle of the cross head is similar to this

Side plate a bit like this

Same plate on the other side to complete

I used the ctr part to base the side plates on onlt needing to enter the diameter of one larger clearance hole and the amount the plate protrudes at the top and its thickness. all other features related to the ctr and will change with it. It also includes the deliberate error that carries from one to the other.

[JasonBModerator @jasonb]

This thread was the previous time we tried to sort out Nigel’s crosshead. Though it is now a 3 piece as post above

[Nigel Graham 2Participant @nigelgraham2]

I tried to edit the drawing but without success.

I managed to change one dimension but not the other, and that on just a rectangular plate with a rectangle of holes for screws.

The crosshead body is much more complicated, and the faults were the width of a recess and the layout of the corresponding screw-holes.

I had already made the real components but mis-measured them for drawing them so I can design their surroundings.

 

I may as well say, “To Hell with formal drawings”, and just use those already done as literal “3D models” plus rough pencil sketches on the backs of the ME&W magazine address-sheets. As I have with some components already.

 

Videos are very variable. Paul Tracey recently sent me very good ones he’d made for TurboCAD.

(TurboCAD’s manufacturer, IMSI, has contracted making tutorial videos to another company. I viewed them but it was obvious the contractor simply publishes a few random ones from three separate series. They are presented very well, but do not transmit to their full lengths [file-size limits?], and the overall result is poor. My impression is that the contractor is purely a third-party technical publisher who does not fully understand the subjects, and with poor oversight from IMSI. IMSI itself now belongs to some outfit not necessarily CAD specialists.)

I did also study the introductory material for Alibre, used in its MEW series.

Generally though, I had been put off a long time ago by “tutorial” videos that were hard to follow; more demonstrations of expertise than instructive.

Also, I find a static manual, printed or in .pdf form, far easier to use than moving pictures anyway.

 

While I am very grateful for all help, I don’t want to rely on deeper informal tuition gambling other people’s valuable time on my abilities. Allegedly I once had an unusually high IQ (by NHS record… even the experts can make mistakes!); but I know I was always a very slow learner with unpredictable but low natural limits for any subject. CAD is no exception, and not alone.

 

I don’t want to adopt yet another CAD system I could no more learn to its full advantage, than TurboCAD Deluxe or Alibre Atom.

Those two differ considerably, and each has its own strengths, limits and level of difficulty quite different from its rival’s. Although I can overlap them enough to be useful, that is not ideal.

If I could, I would use just whichever is the one easier for me, for both single items and assembly drawings.

 

[Nigel Graham 2Participant @nigelgraham2]

Having just seen Jason’s comment above about “unreliable parts”…

There is nothing wrong with the physical cross-heads I made! 

I like his suggested way to make them but I used a pair of castings from the waifs-and-strays tray on M.J. Engineering’s trade-stand. They may originally have been for a 7.25″ g. locomotive, by their shape and being a pair cast in one.

My dimension errors were in the drawings I made of them later, in their finished form. Not on the actual metalwork.

Though I now realise the mistakes would have stopped constraining them together as CAD parts.

 

I have to replace real parts already made far more to improve the design or correct design flaws, than to correct simple metalworking errors.

I had hoped that using CAD would help me design the lot before using up any metal; but no. All it gives me is much quicker and intrinsically more accurate drawing, and easier editing, than by hand. My dimension or shape mistakes on a drawing are nothing to do with how I drew it.

Editing… Well all right, replacing the drawing if I can’t alter it. Which I usually can’t.

Modifying the faulty cross-head body model might have been possible but certainly not easy, and anyway I assumed it useless and deleted it. A copy does exist on a partial assembly and might be salvageable from that. Which makes me wonder if in fact I re-draw the thing at some point, and put the mistakes in the second drawing.

[JasonBModerator @jasonb]

I meant you can’t produce reliable CAD parts. So using one to drive the design of another would just give two parts with errors.

The part file should still be in your recycle bin and can be retrieved from that.

[Nigel Graham 2Participant @nigelgraham2]

Ah, I’d not done it like that.

I’d measured one piece of metal and drawn that. Then I measured the other bit of metal and drew that one.

Only, I’d mis-measured both so both drawings were wrong, and their errors differed. The real bits of metal fit together but the images of them don’t because their mating features differ!

No wonder none of the constraints would work, but that was not obvious to me for a long time.

….

I did try using Alibre again this evening but for something else completely. I have just fitted my Harrison lathe with a boring-table and need make adaptors to use existing tool-posts etc. I needed widen my first sketch of the upper plate, a preliminary design for holding the lathe’s original top-slide (albeit with a big loss of tool height). I still can’t edit a drawing’s dimensions though so had to re-draw it, even though it is just a rectangle with some holes in it. I doubt I created the Tee-slots in the best way either, plotting the initial profile for each, individually. Nor could I work out which planes to use for for the best so the table was the right way up but I had to turn the plate round in two planes. The engraved “F” (front) is not on the real thing. It’s to orientate the drawings.

 

 

 

[JasonBModerator @jasonb]

Dimensions should be easy to alter but could depend on how you have dimensioned the original part. Open the file, right click the sketch of the rectangle you want to alter and select edit. Then take a screen shot and post it here. Better still email me the part file.

As for the tee slots you could have sketched and extrude cut one then used a “linear pattern” to add the rest.

[JasonBModerator @jasonb]

I’m not sure what you have selected but if “toggle sketch dimensions” is clicked then you can see what dimensions you have added during sketching and a double click on any one will allow it to be altered. Atom displays thos elittle icons differently but you should still have that icon somewhere.

[David JuppParticipant @davidjupp51506]

Nigel,

It might help if you send a part file or two where ‘can’t edit dimensions’ to me (or Jason if he’s willing) – then maybe one of us can show how to make the changes.

Atom3D doesn’t offer the option to turn dimensions off in sketches, so that shouldn’t be complicating matters (unless there is a display issue that needs to be resolved).

Whilst most dimensions will be in 2D sketches, some will be held in (for example) the ‘depth’ value of an extrusion, or the repeat distance of a linear pattern.

[Nigel Graham 2Participant @nigelgraham2]

I tried to use the Linear Pattern but could not understand what it wanted. It asks you to enter the direction but I could not fathom what it really wants.

I tried changing the dimensions both in the sketches and in drawings made from the models but found it might work for one and lock others.  I have not deliberately locked anything, but can the dimensions be locked, perhaps even by accident?

[David JuppParticipant @davidjupp51506]

Linear Pattern – ‘Direction’ can be

• an axis
• a straight edge that exists in the part
• normal to a circular edge in the part

2D drawings are driven from the 3D model, so changes in the 3D model will alter the 2D drawing (after re-projection).

In most cases, changing a dimension value in the 2D drawing is not readily done (can be over-ridden), BUT there is one exception.  If you include ‘Design Dimensions’ automatically in your drawing these can be edited and will change both the 3D model and the 2D drawing.

I rarely include Design Dimensions in 2D drawings, because they rarely display in a convenient location.

 

For simplicity, I suggest that you make changes in the 3D model only.  The 2D drawing will prompt you to re-project views due to the changes when next opened.

Avoid having both model and the derived drawing open at the same time – it can lead to much confusion, and potentially to the loss of intended changes.

[JasonBModerator @jasonb]

Direction is what way you want the pattern to replicate in, so in the case of your cross slide you want to replicate along it’s length not up/down or off to one side so I would most likely have picked one of the long top edges.  You then have an option of which way the pattern will run so if you drew the first tee at the front of the slide you would want it to repeat towards the back, if you drew it at the rear then reversing dircection wil put the others towards the front.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou.

 

I tried using an axis for repeating direction but it didn’t seem to help. I might have been using the wrong axis, of course.

It wasn’t hard to replicate each ‘T’ along the block, just rather laborious.

[Nigel Graham 2]

On Nigel Graham 2 Said:

It wasn’t hard to replicate each ‘T’ along the block, just rather laborious.

Also can be error prone, having to replicate the same profile several times.

The big benefit of linear feature pattern comes when you’ve made a mistake (or weren’t sure of a dimension to begin with).  Having a single T profile in a sketch, plus a spacing value in a pattern, makes it very easy to edit the slot profile, spacing, or number of slots to either correct an error, or just to look at options.

I’d almost always advocate using 3D feature pattern over 2D sketch pattern, because subsequent editing is so much easier.

[Nigel Graham 2Participant @nigelgraham2]

I’m afraid I have to use less than ideal methods when I can’t see how to do it properly. It wasn’t easy, plotting all those profiles separately, and I had to correct a few mistakes before extruding them.

I’ve re-drawn that crosshead and this time it went together properly, once I’d turned the cover the right way round. The four screw-holes in each even line up!  The cover as drawn overlaps the ends of the casting a bit, but that’s because the real thing is rather irregular in that area and I used a rough average distance between the edges.

There are two details I did not attempt. On the real metalwork I made two small channels from the top “chisel” edges down to oil-holes at the base of the boss, but decided them too difficult and rather unecessary to draw. On the actual engine these units will reciprocate vertically, so the bevelled edges and oil-channels will collect oil from the guide-bars and feed it to the gudgeon-pin. Well, that’s the aim!

The pin incidentally, is a commercial shoulder-screw with ground shank, intended for purposes like pivots. I have not tried to depict the M6 thread on its projecting end.

[Michael GilliganParticipant @michaelgilligan61133]

Bravo !

MichaelG.

[David JuppParticipant @davidjupp51506]

Nigel,

Very sensible not to attempt thread modelling – it is resource intensive, and hasn’t traditionally been the easiest thing to do.  Most of the time it really is not needed.

For those occasions where modelling the thread really is necessary – it suddenly got much easier with version 28.1 of Atom3D – see from about 1:10 in this video.

https://www.youtube.com/watch?v=0-wH18fAFX0

And even if not needed to be modelled, the ‘cosmetic’ view is handy.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou both!

Detailing ordinary, standard threads (M6 in that case) was not normal drawing-office practice anyway.  It would be necessary only when designing the thread itself, or for illustrating techniques like screw-cutting.

Perhaps it could be represented in 3D CAD by a cylinder of slightly reduced diameter, corresponding to the real thread’s truncated crest? Unless rendered away, its length would show by the “glue line”, too.

 

Since that crosshead, (measured twice, drawn once, this time!) I used Alibre Atom again in designing a riser-block to hold a 4-way tool-post on my Harrison lathe’s boring-table. Only later, realised a feature on the second-hand, tool-post was for some previous use, and would give needless, extra work!

Still, it was a useful exercise… I found how to create a hexagon, and how to use one Part as a template for its companion.

 

The surplus feature is the large hexagonal head on the central pin shown below. That would likely have fitted a T-slotted slide on a particular lathe. My application needs only a simple stud screwed into a single block that lifts the unit to the right height above the table.

The original parts, with the tool-holder’s clamp-screws and handle omitted, are in green.

The shallow holes in the holder’s underside have arcuate entry ramps, forming the ratchet, but they were a bit too hard to model.

As designed here, the riser block (on left) with 4 tapped holes, and the two plates forming the housing, are held together by four M6 socket-screws whose heads, slightly slimmed to fit, would also act as the fixed pawls.

Later I realised I can remove the hexagonal head, dispense with its two-part housing, and put the recess for the tool-holder location-boss, the socket-screw “pawls” (or just plain pins) and simplified central stud, directly in the riser.

I know there is an “Exploded View” tool but could not see how to make it work, and “Search” did not do any searching.  So I just put the bits into an Assembly page and arranged them by eye.

 

 

[David JuppParticipant @davidjupp51506]

Nigel,

Exploded views rely on assembly constraints being in place – these define the directions in which to explode.  If there are not assembly constraints, the explosion won’t have any effect in either Auto explode or Manual explode modes.

It looks as though you are making progress.

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