Member postings for David Jupp

It may be helpful to enable 'Prompt for new file names' in System Options -> All workspaces -> General ; that way you'll get a dialogue allowing you to set name each time you start a new design.

As I've said before - no single 'correct way', and people have their own preferences.

The question related specifically to Atom3D, where toggling grid snaps on/off requires a diversion into System Options, it isn't easily doable from the workspace.

The question was also specific to GRID SNAPS, not other types of snap.

Lee,

Part Scale/Mirror should not cause disappearance. If there is unexpected behaviour either raise a support ticket with Alibre and include the file, or PM me, or in UK contact Mintronics. Depending upon day or week & time of day, I may well pick up the Alibre support ticket, Mintronics support ticket for Alibre products often, but not always come to me.

Trials are available for Atom3D, or Design Expert - there isn't normally a trial for Design Professional, which sits between them - but there is quite a lot of information available on differences. In extremis, a trial could be arranged for Design Professional if needed.

Personally I would say NEVER use Grid Snaps.

I have come across woodworkers for example, who work on the basis that all measurements are multiple of 1/4" or 1/8", and they only ever use right angles, so they find grid snaps can speed up their sketching. Grid snaps do allow you to be rather lazy about defining dimensions, as you are unlikely to accidentally drag a line end (say) away from a grid snap. Maybe helps with making sure lines ends meet, but the non-grid snaps can also do that.

As you've found snaps can cause unexpected problems - so I'd turn them off. If you do come across a case where you decide they'd be really beneficial, you can turn them back on for that project.

Typically the Sales channel for your region will follow up in one way or another. If that doesn't happen for any reason you can of course initiate contact.

At the follow up contact, it's a good idea to ask about any remaining concerns/uncertainties before you make any decision.

Nigel - be VERY careful here - it can all be done, but it's also easy to mess things up badly.

If you change the name of a part file outside of Alibre, this can have dire consequences. Use 'Save As' from inside Atom3D if you want to save a version of the file for archive/fall-back, or to edit it to produce a variant of the design.

For an explanation see this help topic

In Atom 3D, if you need to substitute one part for another in an assembly, you have to delete one and then insert/constrain the other. In higher levels of the software there is 'replace component' tool that can make this a bit easier to achieve.

Edited By David Jupp on 13/05/2023 11:14:48

Edited By David Jupp on 13/05/2023 11:15:08

Lee,

A Mirror operation mirrors the FEATURES, this is often not the same as mirroring the result of previous features. It can end up with everything disappearing if you mirror a cut - you then have 2 cuts removing both halves.

There is a separate Scale/Mirror Part command which can be used to mirror the part completely (or scale it).

Search for 'vacuum feedthrough' - you'll see stuff from a range of manufacturers, and hopefully some outline information on seal types, materials etc.

I'd probably be looking to buy a commercial multi-pin feedthrough and solder wires onto both sides. It gets a bit more interesting if you need coaxial cables to be brought through, but that is possible. My own knowledge is with high pressure, so I'll avoid giving direct recommendations.

Martin,

You didn't change the option - it defaults to Sketch Figure (which is often, but not always, what is needed).

If you get the wrong figure type, simply right click on it and 'Convert to Reference Figure' or 'Convert to Regular Figure' depending upon the offered option.

If number of holes in a pattern might change, use a 3D Feature Pattern instead of a Sketch Pattern to add copies of the seed hole. Similarly if the hole size might change.

Patterns in sketches can't easily be edited if you return to the sketch at a later time. Whereas Feature Patterns can easily be edited - say from 5 to 6 holes. Edit size of circle for seed hole, and other holes created by the Feature Pattern will update too.

Nigel - very sensible to practice simple steps and 'play' with individual tools to build understanding of how they behave. There are several options for even the simplest tools - which can often be glossed over. More complex tools have loads of options and hence many more ways to go wrong!

Edited By David Jupp on 10/05/2023 11:37:06

Dave -

Nothing to do with faces/planes or 'mid-air' - Jason's diagnosis above nailed it.

Sketch was not closed due to containing a circle crossing the long side of the rectangle. If the projection of hole edge had been a reference figure, it would have worked.

Martin did show sketching on the face. Not sure what you mean by 'starting in mid-air'... If you mean on a plane, that is actually 'best practice' in 3D CAD. It is more robust than sketching on a face, but at expense of taking extra time.

If you hadn't already noticed, terminology in CAD has some very specific meanings that may not entirely match everyday usage. Usage of names may even vary a little between different products.

Often a big problem is working out exactly what a user is actually trying to describe if they don't use terminology in quite the same way as we expect.

This is just one reason why getting hold of screenshots, and/or the actual files is so valuable when diagnosing issues.

Nigel,

If grid snaps are on, lines can only start and end on grid nodes, not between them. That's why I never use it (but some people do find it helpful for some kinds of work). With grid snaps on, the angle for taper of the column probably wasn't compatible with the grid.

Very glad to hear you are making better progress now.

Just a note on 'variables' (or parameters) - any dimension that you apply in Atom3D gets a name (which you can alter) and is held in the 'Equation Editor'. Even if a value is not intended to change, you can use it to help define other values in the design. Instead of entering an explicit value, you can set things such as 'D6 = 3 x D3' , then if you alter the value for D3, D6 will also change to satisfy the equation - or you might decide later that 3.5 x D3 gives more pleasing proportions to the eye for the finished part.

Nigel

The snap threshold below the grid settings is for snapping to items other than the grid. See This help section

People can see that we all have our own different habits and preferences. There is no single 'correct' way!

Steve,

Top row are all about grid - Visibility, Snaps (ON/OFF), Grid size settings

Middle row, toggles in turn for DoF Colours, DoF Callouts, Real Time Dimensioning

Bottom Row - Visibility toggles for Dimensions, Constraint Symbols, Guide Lines

You have much more control of exactly what shows up in Pro or Expert, and easier to toggle stuff without jumping to System Options - BUT more to learn and remember.

DoF = Degrees of freedom, whether figures are fully defined or not.

Edited By David Jupp on 09/05/2023 15:51:48

Steve, if you are looking for Grid & Snaps settings they are accessed via 'System Options' - see image. Note that there is another set of Grid options for the 2D Drawing workspace sketching.

The Snap Threshold setting below the Grid Area is for inferential snapping to lines, nodes, axes etc. Have it too small and you have to be extremely precise to select anything, have it too large and it may end up offering items you'd rather not have. Best setting for you may depend somewhat on your screen size/DPI.

Steve,

Jason is using Alibre Design Professional - Atom3D doesn't have the same options on the Sketch Ribbon - it is deliberately simplified.

Nigel,

Send me a part file that you can't drag sketch figures in - I can soon check if this is because figures are fully defined, or if it might be to do with your installation, or your way of working.

Yes. Whichever of root/crest is in middle of profile shouldn't be a problem in the profile sketch - for the other rounding, don't try to put it in the sketch, instead apply a 3D fillet after the helical feature.

If still not clear - submit a support ticket to Alibre and include a part file that exhibits the problem. There is an issue this morning with the cloud service used to handle support tickets - I or a colleague will pick the ticket up when the service is fixed.

The MEW articles mentioned through this thread show one way to form the profile sketch to avoid overlapping.