Member postings for David Jupp

You might be able to download a parts list for it from the Mitutoyo web site

**LINK**

Jason, if having STP can the variant STEP also be allowed? - both are used. Allowing both might be simpler than expecting people to edit the file extension.

Just to expand a little on what has already been mentioned. In 3D CAD, the Exploded View is created and edited in the 3D Assembly workspace. Explosion directions are typically set by the assembly constraints that hold parts together. There may well be an 'Auto-Explode' option, the resulting view can be refined/adjusted manually.

Once the Exploded View is to your liking, it can be added into a 2D drawing. Callout numbers can be added based upon a Bill of Materials (generated automatically from the Assembly).

Some systems allow the explosion to be split into steps, and exported to an animated PDF 'manual' - think of a 'workshop manual' with animated 3D colour images showing assembly or dis-assembly steps. Instructions and animated images are stepped through under control of whoever is viewing the PDF.

Nigel,

Yes I see the sketch and model mirror types' difference.

There is also Sketch Mirror. I was particularly pointing out the different between

FEATURE mirror and PART mirror, both of which work on 3D geometry, rather than sketches.

Nigel,

Your can mirror 3D Features within a part, there is also a tool to scale or mirror the complete part.

Feature Mirror and Part Mirror behave differently - it's important to choose the correct one.

Feature Mirror can add mirrored geometry into the part, whereas Part Mirror will create an 'opposite handed' version of the part (and the original handed part vanishes).

You can edit an existing sketch most reliably by right clicking its name in the Design Explorer (on left of screen), then choose Edit from the context menu. As you've found there are other ways to access an existing sketch.

Nigel,

In almost all cases the 'default grid' in 2D sketch mode is nothing but a distraction - I'd suggest turning it off, so that you get a clearer view of the workspace.

Also unless you specifically want to use it for some reason, make sure 'snap to grid' is disabled.

I believe we covered both these points when I did a screen share with you some while back.

Atom3D does not have 'rectangle by centre' that Jason mentions - BUT there are ways you can work around this.

• Use symmetry constraints in sketch to make rectangle symmetrical about default axes.
• Add a reference line across diagonal of rectangle, add a mid point node on the reference line - you can use that to fix the rectangle to existing geometry.

There are probably other options depending upon the exact circumstance.

Can I suggest that you stop at each of these small roadblocks you hit and submit a query to Alibre support - send in your file with a clear question. Something like 'how do I make the rectangular pattern of circles in sketch 5 be centred on the hole created by Extrude Cut 3?'

Whilst Alibre Support is not a training service, they don't want you to struggle or fail. Don't feel that any question is too basic (you would be surprised at some of the queries that come in).

You can submit support requests at https://support.alibre.com/s/

Edited By David Jupp on 09/08/2023 08:00:03

Edited By David Jupp on 09/08/2023 08:00:59

Nigel,

I could not work out whether you pick the Tangent Constraint then drag the line from the corner to the circle, or the other way round, or what; so when it did work after numerous attempts I had no clear idea what I had done right.

After selecting tangent constraint, follow the on screen hints at bottom left of the Alibre Window - you do not drag, you select in order the items that the constraint should apply to. Ideally the first selected item should be the one you do not want to move.

I thought there should be a "Symmetrical Constraint", or something like it, but failed to find one that offered what I wanted: a single line placed centrally across an axis. So I had to resort to very roundabout ways. The little instruction on the command labelled "Symmetric Constraint" is about two separate objects. The nearest alternative, Midline, didn't seem the right choice either.

You should have applied symmetric to the END NODES on the line, about the central axis. I.E. select symmetry tool, click the symmetry axis, click one end node, then click the other.

It might help us to follow along if you don't use the term 'drawings' to mean everything. In Atom 3D there are 'sketches' - these are profiles and paths which are used to help define 3D features in 'parts'. Parts are saved with the extension AD_PRT

The 'parts' get combined into an 'assembly' if required. Assemblies are saved with extension AD_ASM.

'drawings' are conventional manufacturing 2D drawings, which are produced semi-automatically from your parts or assemblies. 2D Drawings are saved with extension AD_DRW.

Nigel,

"and on the drawing it was visibly not quite concentric with the arc, but we can't have everything."

You can apply concentric constraints within sketches - either between items in the same sketch, or between an item in the sketch and an existing 3D edge

"I traced the cut-outs on frames of reference-lines, one plotted at each end and made symmetrical about the centre-line by dimensions (must be an easier way)."

Yes there is - use symmetric constraints in the sketch. Or mirror the 3D feature once produced. Sketch Mirror is also possible, but has some disadvantages.

"Surely it's not necessary to plot completely the same geometry four times, twice on each half, either."

As Jason has mentioned there is a feature mirror tool. In some cases a feature circular pattern can be an alternative - depends rather on the detail of the part.

Nigel,

Is there any way to leave the holes off the Parts to start with, then extrude them through both Parts in the Assembly? Sort of modifying the Part from the Assembly, not modifying the Assembly by modifying the Part?

In the 'Expert' level of Alibre Design it is possible to create 'assembly holes' - think of 'match drilling'. As with all things there are pros and cons to this method.

Even in Atom3D, you can 'project to sketch' the edges of holes in one part into another part that you are creating or editing in the assembly. This creates an 'inter-design relation' so future edits of one part will update the other.

Drawing even spur gears to full form is too advanced for me...

In Pro and Expert levels of Alibre Design, there is support for scripting, which includes a spur gear generator (it is set up a bit weirdly, but I have some modified versions which may be more useful).

Also (and I just checked that this does work with an Atom3D licence) - an Alibre user has programmed an add-on which produces spur and helical gears as well as as cycloidal gears - it does all the maths for you as well as the modelling. Installing the add-on is not complex, but does require familiarity with copying files into program folders in Windows. If anyone is particularly interested, drop me a PM in first instance.

Even though realistic or even 'correct' gears are possible - they will require a fairly good PC spec to avoid making the system very slow to respond.

Nigel,

Another way to recover from an accidental New Part, is to right click on the New Part in the Design Explorer, then click 'Edit root assembly' - this returns you to the assembly level.

You can now click on New Part (in Design Explorer or the 3D workspace) and press Delete on keyboard.

This page may possibly help **LINK**

Text on curved faces can already be done in Alibre, using the wrap/project tool.

The coming enhancement for v27 is text along curved path. The two things are different, but may sometimes be usefully combined.

Personally (and this is largely preference), I would have used feature pattern instead of sketch pattern for the steam drillings. That way only one circle to edit the size of to re-size hole - and if you actually intended the holes to touch or overlap, you can because the sketch won't have any overlaps.

There are usually several different options possible for any particular modelling task.

Edited By David Jupp on 18/05/2023 10:51:37

Posted by Nigel Graham 2 on 18/05/2023 09:36:00:

Sorry - I'm not sure how you make something symmetrical as you say. I had turned the Grid and Grid Snap off as advised, and that makes the starting rectangle aligned with the grid but not the big dot in the middle. So had to place everything by dimensions from the edges.

You can use dimensions, but more effective is to use a symmetry constraint in the sketch

However, I found it very hard to calculate the sizes of the cutting rectangles for the HP side, leading first to biting into the block on both sides of the cylinder, then landing short so I had to take a second extruded cut at it. I think this is why the drillings on that side bite into the port wall. I could not make the holes tangential to the right edge, due to having two slightly overlapping sketches.

Rather than take second extrude cut, edit the sketch or depth for the first one to change its size.

If overlapping sketches is confusing - Toggle Sketches off on View Tab of the Ribbon. Then you'll only see the sketch that you are currently editing.

I tried to remove the faulty sketch lines but couldn't, so how do I do that?

Edit the sketch containing the lines, select line or lines, then either press Delete key on keyboard, or click the Delete symbol on the pop up window. Alternatively, right click the line, and select Delete from the context menu.

It would seem to use CAD efficiently without mistakes hard to put right, needs planning the drawing order, often but not necessarily always the physical making order.

There is an element of that. Also be aware that if you get the order 'wrong', it is possible to move items around in the Design Explorer to change the order afterwards. If you do that always press F5 to regenerate the part as this should highlight any failures that the change of order has lead to. Because features are built each one 'on top of' earlier features, changing the execution order can lead to problems, so proceed with caution.

Edited By David Jupp on 18/05/2023 10:11:01

Nigel - is that just an unfortunate phrasing / typographic error, or are you modelling the features at scale, rather than at actual size?

It is usual practice to model everything at actual size, then let the software take care of producing scaled views in any 2D drawings.

Use of section views in the model, or setting the part semi transparent, can be really helpful to see where holes get too close for comfort.

The upgraded text tool for Alibre v27 (taken from a post by Alibre CEO on Alibre's user forum)

Lee -

Another option, DeskEngrave (an old piece of free software) can provide a way to do text on curves and transfer to CAD via DXF.

As mentioned, from Alibre v27, Jason will be able to do his curved text much more easily.

I'm told that 'text along a path' should be available in all software levels in version 27. There's perhaps a small chance that could change before release.

Jason did all those nameplates the laborious way, placing each letter individually.  He uses Alibre Design Professional, but text tools same in all levels.

Edited By David Jupp on 16/05/2023 21:32:20

Text tool in Alibre Design / Atom3D is relatively basic. There are some extra abilities being added for the next release due later this year. Should help with doing things more complex than straight lines of text.

Ady,

When you make a new part 'in context' of the assembly, the part workspace shares reference geometry with the assembly. Will only be able to move the new part when you return to editing the assembly, and depending upon exactly how you modelled the part - movement can be restricted if you used geometry from other parts to define it.