Learning CAD with Alibre Atom3D

[JasonBModerator @jasonb]

I did also find an easier way to set the angle of the sketch. Select dimension and then just click the top edge of the knob and one long side of the sketch and enter the desired angle which seems far simpler than the method suggested.

Could also have been done at the time of drawing the first line by just hitting tab and entering the angle.

Edited By JasonB on 29/01/2019 19:14:05

[David JuppParticipant @davidjupp51506]

I just took a look at the Alibre web site – there are some new videos specifically covering Atom3D that have been added to the training area. Make sure to look on the Atom3D tab, at time of writing the videos on the Alibre Design tab are still rather dated.

[John HinkleyParticipant @johnhinkley26699]

Taking yet another break from my engine design, I've been pondering the question of a simple indexer. I have come up with a prototype as shown below, modelled in AA3D

At the moment, there is no spindle shown as I haven't got around to drawing it, but the intention is to use a commercial ER25 chuck with 100mm straight shaft – because I happen to have one. It operates on the following principle: (Skip this bit if of no interest!)

The outer,lefthand, disc is key to the shaft so that it rotes the workpiece as indexing progresses There are holes drilled in it at specific angles, such that by inserting a dowel in each hole in turn, it engages with a similar hole in the next plate with holes at the same angle plus one degree. The other side of the second plate has holes at 10° intervals and the engraved register allows one to set the second index position at a specific number of 10° intervals and the first plate adds the second and subsequent indices.

It will only allow whole degrees to be indexed, but could be useful in instances where that is all that is required.

I need to find a local foundry that will cast me a body from a pattern I'll have to make!

More progress will appear in the album, not here.

The design is in a state of flux and I will incorporate "improvements" as and when they occur to me!

John

[Neil WyattModerator @neilwyatt]

That makes me think it would be great to have a design for a multi-purpose casting that could be used for spindles, indexers, tailstocks. Something like an cylinder on an angle plate so it could be fixed on its side or on its end, with a couple of mounting points on the cylinder.

There could be a challenge to come up with the most flexible casting, and then for different things to do with it. Might even be popular enough for someone to sell it for a reasonable cost.

Neil

[Kenneth Jones 1Participant @kennethjones1]

Hi Neil & David,

I am up to Fig 47 but try as I might the thread does not appear. I get the ghost thread as in B but when I click 'apply' it all disappears.

I have checked on 'status' and it tells me;- 9002 open or overlapping figures are not supported.

I can not see what I am doing wrong but you say make the height 6 but the part is only 5 thick, is this correct? I have selected 'Height and Pitch'

I am quite proud of my progress so far!

Thanks. Kenj

[David JuppParticipant @davidjupp51506]

6 is correct –  in fig 46 the sketch profile for the groove of the thread is drawn just outside the thickness of the part, so the cut needs to extend a bit further than the thickness to make sure the thread goes all the way through.

Open or overlapping figures suggests either a gap in your sketch profile (use the sketch analysis tool to check), or the profile is wide enough that adjacent 'turns' will overlap (that causes problems) – so axial width of the groove profile must be less than the pitch value.

This might help.

Edited By David Jupp on 01/02/2019 17:01:33

Edited By David Jupp on 01/02/2019 17:07:12

Edited By David Jupp on 01/02/2019 17:08:36

[Kenneth Jones 1Participant @kennethjones1]

Thanks David, — but still no thread!

I can not locate 'sketch analysis tool'

I did look at your suggested help tutorial and my problem does suggest a fault in the sketch as I have tried different shapes (rectangles and circles) and I can make a spiral cut using these shapes. I have also tried changing the pitch, that works on my simple shapes but not on the thread shape (triangle).

Am I right in thinking that the groove profile is 2 x 0.375 =0.75, there for less than the 1.0 pitch suggested so that should be OK

Am I the only one having this difficulty?

Thanks'

kenj

[David JuppParticipant @davidjupp51506]

Ken, In System Options -> Parts/Assemblies -> Sketching, make sure that the check box for 'automatically analyze sketch' is indeed checked.

If still struggling, let me know.

You may have one line on top of another in your sketch (hence 'overlapping' ).

 

Edited By JasonB on 04/02/2019 08:29:48

[Kenneth Jones 1Participant @kennethjones1]

Hi Dave,

I'm there! I switched on the sketch analysis button as suggested and tried yet again.

The analysis did indeed suggest that I had an open sketch in spite of very careful location of my curser!

BUT, I tried deleting the vertical line, ie; the back of the triangle, and low and behold the thread then appeared.

I am at a loss to explain this but it has worked for me.

Thanks again, I am looking forward to next months tutorial.

Cheers, Kenj

[David JuppParticipant @davidjupp51506]

Ken – perhaps you missed out this step (my bold);-

Change the right hand edge of the triangle
to a reference figure (this option is found
under the right click menu), then extend the
shape with the line tool and set the distance
to 0.2mm as shown in Fig 45.

A reference figure is like a 'construction line' – it is ignored for the actual extrusion (or other feature).

[mickParticipant @mick65121]

Back to playing with the cylinder head. How do I anchor the 12mm diameter sketch to the top face of the head in order to extrude it to form a counter bore. Thanks.

[David JuppParticipant @davidjupp51506]

Mick – the first step in creating any sketch is to choose a plane OR a flat face to sketch on. So in this case, and assuming the top of the head if indeed flat, select the head top face, enter 2D sketch mode, place 12mm dia circle and constrain concentric to one of the existing holes.

If the top of the head isn't flat, you'll have to add a new plane at a suitable height to start your counterbore from (that could be just above the top of the hole, or it could be at the level you want the bottom of the counterbore to be at – the direction of cut will be opposite for these 2 options.

[JasonBModerator @jasonb]

Looks like you have also selected extrude but if it's a counter bore you want "cut extrude" to remove metal.

[Kenneth Jones 1Participant @kennethjones1]

Of course, now the penny has finally dropped. The tutorials were banging on about crossing lines and I was not taking it in. I may have learned the hard way but at least I have learnt.

Thanks Guy's

Kenj

[George ArcherParticipant @georgearcher16419]

I am very grateful to Jason B for his "get round" to put the angle on the rim of the thumbscrew. However I tried the dimension would only produce a linear distance. It appeared the system did not recognise the axis as an element in the drawing. Does Alibre have a digital "foremans boot" perhaps by keyboard shortcuts to encourage the system to do as its told?

[JasonBModerator @jasonb]

Sounds like you may be clicking on the line that defines the edge of a plane rather than an axis. if you hold down both mouse keys and drag the part slightly you should be able to see if it is that or an axis line you are selecting to dimension from.

[mickParticipant @mick65121]

I've been playing with different approaches the past couple of evenings without a lot of success, so suggestions please on the method of generating cooling fins on the top of the cylinder head, I'm not concerned if there're vertical or horizontal. Thanks

[JasonBModerator @jasonb]

Horizontal would have best been done at an early stage where a section through the head sketched out and then rotated. Though you could do a cut rotate to get the same result without having to go back to the start. Draw on the XY plane and then rotate about the Z axis. You only need the sketch to be half the head.

vertical fins can be drawn on the XY or YZ plane and then use cut extrude and select "through all"

If not sure let me know and I'll post a couple of examples later.

[John HinkleyParticipant @johnhinkley26699]

Help!!!

This morning, I opened AA3D to continue working on some drawings and got the message that "License ( sic ) initialisation was unsuccessful. Error code 10000442". Tried again, this time error code ended 514. then again, ending 550. In desperation, I downloaded the program again, uninstalled the original ( ver 2 ) and re-installed. This time the error code ended 496. Undaunted, I tried again, now the error code ended 333. Next try ended 553.

Now I am daunted. Please don't tell me I've lost access to all the work I've put in over the last 3½ monhs since I started using the trial.

Anyone got any ideas? And, yes, I know I could contact support, but I'd like to get it sorted PDQ.

Thanks,

John

[David JuppParticipant @davidjupp51506]

John – fear not. This article will show you how to fix it.

You will need to re-enter your activation code – if you can't find it, contact support (they can find it from the details used when setting up the trial).

Edited By David Jupp on 08/02/2019 10:27:07

[John HinkleyParticipant @johnhinkley26699]

Thank you, David. I remembered seeing that tip somewhere before, but failed to find it in this thread. I'll try it now and report back.

John

………. Just a few moments later and I can start breathing, again. All back to normal, thank goodness. Many thanks for your help, David.

[David JuppParticipant @davidjupp51506]

Boring technical explanation – communication between your PC and the Licensing server involves an 'offset' parameter. This changes regularly and is remembered on your computer. Should the offset value get 'out of synch', all communication becomes garbled. Deleting the local licence copy (which is what that article details an easy way of doing) re-sets communications and establishes a new offset value for future communications.

[mickParticipant @mick65121]

Hi Jason. I've drawn another sketch but can't exactly see the way forward. If you could, when you have the tine, give me a view of the section and the cut rotation you mentioned it would be appreciated. Thanks.

[JasonBModerator @jasonb]

Will post it after dinner, I have done the sketche salready.

[JasonBModerator @jasonb]

So as I said before I would draw a sketch and rotate that to get the basic shape of the head.

Which when rotated gives something like this

First option to add horixontal fins would be to incorporate them into the sketch shown above which would then look something like this

And when rotated gives this result

If you don't have a sketch like mine or just want to cut the fins into your existing head then a sketch can be drawn where the cuts will be. Notice that I just drew one 3mm high rectangle and then used the linear pattern tool to place the three others above that rather than draw out the whole lot.

Then using the revolve cut about the central axis the slots can be cut out, they first show as the blue guide lines

But once you click OK they will be cut out like so.

If you prefer vertical fins then click one of the vertical planes and draw the slots on that, again I drew one slot and then used the linear pattern for the rest. Decided to just draw slots through half the head so I could avoid the valve holes

Then used cut extrude and selected through all

After clicking OK it shows the cuts as on the left below. Then to slot the other side I used Mirror to get the other cuts shown as blue until OK is pressed.

Then you get to see the finished cuts

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