Learning CAD with Alibre Atom3D

[JasonBModerator @jasonb]

(i) It won't work in Atom as you would have needed to put in the thread details during the 3D stage to be able to have it available to call up on the 2D drawing and it is not a feature that AA has.

(ii) I will leave that to David

Best bet would be to draw tapping size circle and then cut extrude that to show a hole in your part. Then when you come to the 2D drawing use Note with show leader (arrow)

Top call out is what the other Alibre versions produce, bottom was done as I describe above

Edited By JasonB on 30/10/2018 07:32:22

[David JuppParticipant @davidjupp51506]

As Jason says – the 'Hole Tool' is not available in Atom3D. Stripping unsupported items out of the UI consistently across all modes has been a far trickier task than I think anyone expected.

I have just checked – one thing that might occasionally be useful – you can successfully turn on hole callouts in Atom3D for a file produced in a version of Alibre Design that supports the Hole Tool.

The wording in the Help may not be the clearest – the content of the hole callout is generated from information in the hole definition (in the 3D model), it isn't created as such in the 2D workspace.

I'll mention this UI inconsistency to the senior team at Alibre. Thanks for the feedback.

[Lionel PullumParticipant @lionelpullum53107]

Thanks guys for the super fast response. Thats what I had imagined would be the case, and I will use the Note feature

[Dennis DParticipant @dennisd]

I am a first time user of any cad package and am enjoying at 70 learning something new.

While waiting for the next tutorial in MEW I came across the exercise manual that comes with the package. Drawing circles is easy as a box comes up allowing you to input the required diameter (manual written for the US so dims are imperial but AA3D converts to metric) but not with a rectangle you need to watch the dimension coordinates to get the size you want.

Way I do it is to draw a rectangle then click on DIMENSION then click the cursor on the side I want to adjust I then move to one side and click again and now a box appears with the length drawn I can overtype it to get the size needed. I then have to select the dims line and right click to get a delete option. Is this the way to do it or have I missed something in a drop down menu.

Dennis

[David JuppParticipant @davidjupp51506]

Dennis, I'm not clear why you would want to delete a dimension after placing it.

You are correct that the rectangle tools don't offer 'real time dimensioning' – you should use the Dimension tool exactly as you describe to size the rectangle. You would normally leave the dimension in place so that the feature can't be accidentally changed.

[JasonBModerator @jasonb]

That is the way I draw them the size them but not sure why you are deleting the dimension afterwards, is it so it does not show on the sketch? If you do delete delete a dimension (constraint) then that line has no fixed length and may move when you don't want it to.

It is possible to set things so that the dimension lines don't show up on the drawing but I prefer to have them showing.

Likewise you can set the default dimension units and decimal places but can also enter other units eg if default is imperial you just enter 1 or .5 no need for " at the end but if you want to draw a metric hole you can just enter 1mm and you get a 1mm hole though it will dimension it in imperial, no need to enter 0.039"

Edited By JasonB on 30/10/2018 10:45:55

[Dennis DParticipant @dennisd]

Thanks for that. I was deleting the dimension to avoid cluttering up the sketch as I progress I will have another go leaving them in place to see the difference.

[David JuppParticipant @davidjupp51506]

Avoiding sketch clutter is a good idea. Best way to do this is to keep the sketch VERY simple. People switching from 2D tend to put lots of things into a single sketch – that will work, but becomes a pain if you ever want to edit things. Much better to use more, simpler sketches to build up the features of the part.

Personally I find Grid another cluttering distraction – so I turn Grid and Snaps OFF.

[Neil WyattModerator @neilwyatt]

Just to add to what David says.

It's very easy to do a lot of work on a single sketch. I rapidly learned it was best to keep each sketch as simple as possible. The part view is uncluttered by the guidelines and dimensions for each sketch.

An exception is doing something like placing several holes in panel where you can use one sketch to place and dimension them so they match up and are aligned, where it can be useful to have them all dimensioned on the same sketch. In this case 'constraints' make life easier.

For example to cerate several identical rectangular cutouts dimension the first one and then use the '=' constraint to make the rest identical to the first one. You can also use other constraints to line them up with minimum need for dimensions. If you then make the first cutout a different size the change will automatically adjust all the others.

Neil

[David JuppParticipant @davidjupp51506]

If in Neil's example the rectangular cut-outs are regularly spaced, you can simplify even further by just having one rectangle in the sketch – cut the hole, then use feature pattern tools (not sketch pattern) to generate the others.

[JasonBModerator @jasonb]

You can also drag any dimensions to where they are well out of the way of the actual work area of the sketch

[Anonymous]

I'd agree with keeping sketches simple. Too many features in one sketch may well be a problem later if you want to change things. You may get the dreaded "Target not available" message, which I'm sure David can elaborate on.

Many of my sketches contain only one item. For instance if I'm creating a PCB for form and fit reasons the outline of the PCB will be one sketch and mounting holes will be another, so they're completely independent. Ok, not quite true as I use Alibre Expert (the program that is, not the user) so I have the "hole" function available, but the point is the same. Things like fillets and chamfers on the PCB would be added later, not included in the initial sketch.

I don't sweat dimensions and constraints to start with; I just draw a sketch roughly where I want it and the extrude. I then sketch, extrude or cut and so on until I've got the basic part. Then I will go back to the first sketch and start adding constraints and dimensions and so on through the design. Finally I'll add things like chamfers, fillets and external threads.

I wondered why Neil didn't use the pattern function. I assumed it wasn't available in Atom. I use the function a lot, both linear and circular patterns. If nothing else if I put all the items in one sketch I'd forget which one it was that I'd dimensioned. I also use the mirror function a lot. No point in creating both sides of a part that has plane symmetry.

Andrew

[Neil WyattModerator @neilwyatt]

Posted by Andrew Johnston on 30/10/2018 13:24:25:

I wondered why Neil didn't use the pattern function.

Because the holes aren't arranged in a regular pattern, but some of the spacings are consistent.

Neil

[Neil WyattModerator @neilwyatt]

Here you go.

The positions of the power socket cutouts are not regular and relates both to the size and position of the large cutout (for a temperature control module which only ahs a about 1mm of tolerance as otherwise it will conflict with mounting brackets for the internal PSU) and each other.

Perhaps the dual USB cutout should be a separate sketch an no doubt it could be done more elegantly, but it was so easy to set out like this, why worry?.

[David JuppParticipant @davidjupp51506]

There is no single 'correct' approach – if it works for you then fine. Here is another way to tackle Neil's power outlet cut-outs, using a single rectangle in the sketch.

[John HinkleyParticipant @johnhinkley26699]

And, just to prove that it can be learnt quite quickly, albeit with a fair bit of help, here's a couple of parts I modelled earlier:

From my album,

John

[JasonBModerator @jasonb]

Looking good John, its going to be quite a big engine

[Neil WyattModerator @neilwyatt]

Well done John.

[JasonBModerator @jasonb]

As David says there are several ways to end up with the same part, for example the base part in the mag article could have been done with just one sketch that was revolved. Though the way it was built up in the article is a better way to show the absolute beginner the basic first steps.

[ZanParticipant @zan]

Assembly problem

Items…..A block housing bearing and shaft

The housing with a hole is anchored on X..Y plane in X direction

A bearing is mated with the shaft

Bearing is mated into the block. All looks good

Colicky the mouse on any menu or in workspace and the bearing and shaft assembly move out still aligned and mated but  always in the same direction, y –

Tried several times, same problem any ideas?

2) is it possible to move the position of the tool groups on the main ribbon bar?

3 is the rendering and reflections seen in Alibra’s web site an extra?

4 what will be the actual cost, to buy at the start and will it need an annual subscription?

5) with mirror  for a symmetrical component, is there a shortcut to select the whole body having created the first half rather than having to select each feature?

Edited By Zan on 01/11/2018 22:38:58 no 5 added

 

Edited By Zan on 01/11/2018 22:42:45

[Lionel PullumParticipant @lionelpullum53107]

Just a tip or two on creating custom templates for drawing sheets etc. To create a custom template follow the help file entry "Changing custom templates" to create your version. You are then free to modify this to include what you do and don't need. But the method to create fields in the description block on your drawing as described in the on-line, is not supported in AA3D. Do not despair, you can get around this with a simple copy and paste. Copy and paste a field title, placing it where you want and double clicking on it to edit it to what you want it to say. Then copy and paste one of the predefined fields, e.g. "Sheet scale" to where you want that. Double clicking on this will open the field editing dialog. At the top of this dialog are two radio buttons, "User input" and "Property value", the latter being selected. If you keep it as this you can select what Property value will be automatically writen into the field from the drop down list. If you select "User Input" two fields, the Name of the property you want to add and a suitable input text string. I strongly recommend using Alibre's format of keeping user defined fields in upper case, it helps when you come to fill in the fields, when creating a drawing, to see which fields need your input. And there you are. Save your drawing template, and when you select in when creating a drawing, you will see all of the fields that are contained in your drawing.

Now comes the hard part – discipline. When you create a model fill in the Properties dialogs, accessible from the jewel icon, with the info thats important to you, e.g. the material. Then when it comes to creating a drawing of the model most of the fields will be automatically filled for you by magic.

Hmm havent worked out how to attach a file or screen dump to this, but when I can I will happily post a simple example

[JasonBModerator @jasonb]

Zan,

1, First I would align the bore of the block with the outside of the bearing. Then if the bearing is flush with the side of the block align those two, if it sticks out then you can enter a dimension. Next align the bore of the bearing with the OD of the shaft and then use mate or align to set how far you want it to stick out.

You will mow be able to rotate the shaft in the bearing but it won't move sideways as you have constrained the sideways positions

 

2, Leave to David

3. You need the Expert version with Keyshot to render but as mentioned in the article ( i think) Simlab Lite is free.

4.£199 one off or £279 with support in UK or see local agent.

5. David again

Edited By JasonB on 02/11/2018 07:04:07

[John HinkleyParticipant @johnhinkley26699]

Just to follow up Jason's comment on Simlab Lite (I have no knowledge of this product ), to obtain the rendered images that I showed in my earlier posts, I first scaled the part in the Atom3D window and oriented it how I wanted it to display, then the file was "Export [ed] to PDF" from the File tab. This brings up the picture in your pdf program – Acrobat in my case – a single click on the picture gives a rendered and fully rotatable version. Take a screenshot and clip to the size and content required. A bit long-winded, but it is a work-around and not something I would do on a regular basis.

I off to investigate Simlab Lite.

John

[JasonBModerator @jasonb]

I export at a STEP file and open that in the rendering prog.That way yo can render individual parts or just one face.

[David JuppParticipant @davidjupp51506]

Zan,

Item 2) – No you can't re-arrange the Ribbon.

Item 4) – Atom3D is sold without 'tech support' subscription (except for licensing and activation problems) – this is to keep the cost down. You can choose to pay (or not) a fee for software updates only. The UK re-seller support option is a special to give new users extra assistance if required (totally optional).

Item 5) – With FEATURE mirror, you have to select each feature that you wish to mirror (no shortcut for all features so far). PART scale or mirror can mirror the entire part. Note that it behaves differently in that it does not leave the original in place. The 2 mirror functions are used for different tasks.

[Author]

Posts