Learning CAD with Alibre Atom3D

A bit fuzzy but will do for now. I am using a different Alibre so the icons are laid out differently but are all teh same as Atom.

I have also put a 1/4" hole in the part to show you can work in imperial and metric and also added small chamfers to the other external edges. I tried to go a bit slowly so the drop downs show up. Watch in You-tube at full screen size.

Jason,

Before I throw in the towel, do you have time to explain how I can edit the dimensions of a circle in sketch mode, including the centre position? All I get when I select a drawn circle and the dimension tool is the diameter of said circle. Nowhere can I get the centre co-ordinates as shown in your screen shot. There doesn't seem to be any way to edit the entity's properties. (I'm using the nomenclature which I'm used to in my present 2D CAD package. )

Thanks,

John

John,

Look at the second photo in my post of 28/10/2018 20:46:13

Place a dimension from the centre point of circle to some other geometry that you wish to set its distance from (for example an axis).

Click the dimension tool icon, click circle centre, click other geometry, move mouse to where you would like to position the dimension, click again to fix that position. Type in the value for the dimension, then click the green tick, or just press return.

Does that help?

Edited By David Jupp on 29/10/2018 12:38:23

Edited By David Jupp on 29/10/2018 12:38:36

John. I'll have a look this evening but is it possible for you to post a screen shot (whole screen) of the circle in question.

For more detail on sketch dimensioning - try this video

First, make sure you are editing the sketch you want to move.

Double click the dimension number with the select tool and you can edit it to what you want.

Position the centre by applying (and changing if necessary) dimensions from other objects edges or reference points, or from planes/axes within your drawing.

Neil

Neil, there is no dimension to edit but I think I can see John's problem.

Edited By JasonB on 29/10/2018 15:15:27

A quick update to pre-empt any further replies. Thanks to the help given by David, Neil and Jason I have cracked this problem. Now to move on to the next one ............

Thanks to all.

John

Hmm new to this package, but I note that you can "turn on" hole call outs in the 2D drawing module (either through the system prefs or clicking on a view and selecting Manage View), but having done that I have no idea how to use it, or whether it is implemented. Reading the help file it says that you must first create a threaded hole with the Hole tool in the thread group which is not an option in AA3D, but that you can manually create a call out by right clicking a hole in the 2D drawing and chosing Insert Hole Callout - this option is not offered either with or without the sketch mode activated. So my questions are (i) am I just being an idiot, (ii) is this feature implemented in AA3D and if not why does is appear in the GUI?

(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

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.

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

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

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.

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

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.

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.

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

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.

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