Learning CAD with Alibre Atom3D

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.

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

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

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?

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.

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

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.

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

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

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.

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.

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.

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

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

For the counter bores that you asked about earlier first click the flat top of the head which will make it blue then activate 2D sketch

Draw a circle roughly over one of the through holes and dimension it's diameter, then using the concentric constraint click the through hole followed by the circle just drawn which will place it centrally over the through hole.

You could do the same for the other 3 counter bored or as I did use the circular pattern feature to place them.

De-acivate the sketch and then use cut extrude, you can either set a depth or if the fins have been drawn already select "to geometry" and click the bottom of one of the vertical slots as the place the counter bore will end.

Click OK and jobs done

You can see I have a lot less sketches at the side than your screen shot, the pale grey pair are the horizontal fins which I have suppressed as we don't need both

Edited By JasonB on 10/02/2019 19:14:55

Thanks Jason, that will keep me quiet for a bit!!

Mick - I'd add that in each of Jason's examples, an alternative approach would have been a single slot profile in the sketch, extrude cut that, then feature pattern to get the required number and spacing of slots.

There is no 'right' or 'wrong' method - using feature patterns keeps the sketch simpler, hence easier to edit.

Hi. Jason, its been far too quiet of late! I've been trying all the methods you've demonstrated but I can't get the results in your screen shots. My screen shots are in reverse order ( can't even get that right!) With the sketch I've produced I get the warning that the sketch isn't closed when I exit sketching. The sketch will only rotate when the Y axis is selected, screen shot two, if I select either X or Z I get the result shown in screen shot 3 and that's before I click the okay tab. When I click okay on the rotated sketch I get the result shown in screen shot 3

You need a horizontal line from ctr axis out to the edge of the head and a vertical line up the central axis which will close the sketch. If you look at my sketch again you can see these two lines, bottom one is red and vertical is orange hence a bit harder to see over the green axis line

For more detail about 'closed' profiles - review this video.