Learning CAD with Alibre Atom3D

Tool - in Alibre a sketch is used as the beginning of making a 3D part. The 2D sketch on it's own in a part workspace won't print because it has no volume. You have to turn it into 3D by extruding (for example).

You can actually print a 2D item -n but only if you create it in the 2D drawing workspace, and use 'sketch on sheet'.

Alibre is a Solid Modelling program, it is optimised for producing drawings from those models, it isn't really intended as a standalone 2D drawing tool.

If you just want a quick sketch to take down to the workshop you can just select print when in 2D sketching and that will print out the sketch as it appears on the screen which can be handy as the green construction lines can be included which can be handy to layout the drawing on metal.

This one I selected print and then a pdf writer rather than a paper printer but both work.

Thanks for your quick reply David. It was an sheet ali disc so I can extrude it by the sheet thickness and all should be well..

Tool

Having gone through the process of drawing the Clamp part I find that I have a dimension wrong, The 6,2mm hole centre is only 8,8mm from the 10mm hole centre. It should be 10mm. Can I go back and just change that dimension and have the rest of the drawing update to suit the adjusted dimension ?

Yes, just make the change, exit 2d sketch mode, then click on regenerate to last feature....any subsequent feature affected by the changed sketch will update automatically.

This is one of the capabilities of A3D that can be a huge time saver. 

A good example is the design of the turbine wheel I posted back on page 23. Getting into the nozzle flow calculations, I found it necessary to increase the blade area by 50%. This involved three changes:

1. edit the sketch for the extrude buss of the rotor OD
2. edit the sketch for the extrude cut for the reversing sector clearance
3. edit the circular pattern to reduce the number of blades in the row by one to provide necessary blade to blade clearance.

Three simple edits that only took a couple minutes....then hit generate to last feature to create updated design.

Edited By Tim Taylor 2 on 21/01/2019 15:58:40

Nige - to expand a bit...

In the Design Explorer (on the left), find the sketch that defines the hole you wish to move, right click on the sketch name and choose Edit. This should re-open the sketch in editing mode. You can double click on any dimension to re-open it and modify.

You can also get into sketch edit mode by double clicking on the face that the sketch defines - though it isn't always obvious if you are on the 'correct side' of part for this to work.

As Tim mentioned, remember to generate to last feature (the button, drag the 'dog bone' down the design explorer, or press F5) after exiting sketch mode.

This is one of the biggest benefits of such a system - corrections or design changes are very simple to perform.

Edited By David Jupp on 21/01/2019 15:49:14

Am I right in thinking that you can't export files in dxf or dwg format from Atom3D? I have searched and can only find references to Alibre Design. Alternatively, how do I get dimensioned drawings printed out. I should say that, up 'til now, I have dimensioned sketches to position lines, circles etc to "make"a part, then deleted the dims to tidy up the sketch. I presume this is wrong. I'll have to improve my dimension positioning to keep the drawing tidy. While I'm at it, I followed Jason's tip to produce workshop drawings ( with dimensions ) but the figures are distorted and difficult to read. Font size 10pt Arial. Over to you ...........

John

John,

Yes it will export:

1. Open the part
2. click on the jewel in upper left corner, then new/new drawing to create a 2D drawing
3. select the drawing parameters and views to create the drawing - you can edit or add additional dimensions at this point......
4. click on the jewel and click on export to export to common CAD format (DXF or DWG)

Edited By Tim Taylor 2 on 21/01/2019 16:17:05

Thank you, Tim. I'll give it a go.

John

John - you seem to be confusing Sketches with 2D Drawings - they are not the same thing. Please don't delete dimensions from sketches, that makes the size no longer fixed and can lead to problems.

If you followed tutorial 3, fig 27 onwards deals with creating 2D drawings from your parts (these 2D files can be exported to DXF or DWG).

Edited By David Jupp on 21/01/2019 16:24:34

Edited By David Jupp on 21/01/2019 16:29:09

John first you need to created a drawing so from the opening Atom window select the far right "Create detailed manufacturing drawings of your design" and from that select paper size and then browse to find the part.

You can also select more options and tick the "use design dimensions" but I prefer to lave that blank and just add my own in a tidy way on the final drawing rather than worry too much while sketching.

Font size and style can be changed when in the drawing by clicking "dimension Styles" and picking "Text" from the list on the left of the window that opens. You can also set the units and decimal places from here too.

Once you have the drawing you can export that as DXF or DWG

Tim,

I did. It worked. Thanks, again.

John

Jason,

Either way works - yours is probably more formally correct.. Personally, since I save related part designs in project sub-directories, I find it easier for me just to open the part first, rather than having to go searching for it. I also tend to generate the drawings immediately after I finish and verify the design, so I already have the part open anyway.

I agree with you on dimensions - I prefer to add them on the 2D drawing as well.......

Tim

@Tim @David

Thank you Guys, that sorted out the problem. Am I right in thinking that to get the Drawing corrected I will have to Re-create it as a New Drawing @

No, you only need to alter the initial sketch, generate to last and then save the part. Next time you open up a drawing or assembly the alteration will be carried through.

If you have the drawing open then save and close it then open up again to get the updated version, it may well highlight the altered part/dimension in red when you first open the drawing.

Edited By JasonB on 21/01/2019 18:59:34

Nige, if you already have the 2D drawing open and have saved changes in the corresponding 3D part, you can force a 're-project views' in the drawing - just a little quicker than closing and re-opening (when you'll be prompted to re-project views anyway.

@David. Thank you so much, that is awesome. Went back and opened the part and when I went to open the drawing the option to re-project was there and accepting defaults in there re-drew it.

Trying to project a slot down the sloping face of a rhomboid figure but instead of following the 'plane' of the face the projection follows the relevant drawing plane as in the screenshot below. Question is how do I most easily acheive what I am trying to do please?

Thought I'd posted a reply - but it's disappeared - so here it is again.

Tim/Jason/David,

Thank you for all the useful tips on dimensions. I really ought to read the tutorials, didn't I? Off to do that right now.

John

Nige you either need to create a new plane at right angles to your sloping face which you can then draw the sketch onto and then extrude cut.

Or select the sloping face and draw a long rectangle on it to represent the width of the slot and then cut extrude to depth, the rectangle will need to project beyond the obtuse angled end