Alibre - A First Attempt

Did you not just make a cover with a right angled cutout then put it all together in assembly?

It will attach at any angle you want

Try drawing it in a single file and you'll go bodmin getting there

Edited By Ady1 on 08/05/2023 03:27:22

Assuming you know the ctr distance between the two cylinders and the stud PCD then that should be all that is needed. Is it a compound or double high? As teh cylinder would likely have been drawn first the cover dimensions could have been taken from that.

Your problem with placing the dimensions all along the axis is either not picking the right two points or simply poor mouse control, Atom will place the dims where you click so after clicking the two points move the mouse away and then click to enter the dimension.

Here is one way to draw it, I have done it with each feature as a separate 2D sketch so it is simpler to follow though several could have been combined eg overall circle, holes and the cut edge.

Recess and spigot are just circles drawn on the surface or plane and extruded or cut as needed

You can see that the box to enter the dimension in can be placed where ever the user wants and I drag it about quite a bit to show that. Then when entering the position of the hole I show what happens if you just click after defining the two points - the dim gets added between the two. I then delete that amd do it again but move my mouse out of teh area of the part.

Also notice I enter the dimension as 60/2 because I want the radius but am using a 60mm PCD

Finally what was learnt on the scribing block exercise can be put to use for creating the cut off edge. I use "project to sketch" selecting one of the hole sand that gives me it's ctr point. I can then constrain the rectange to that and cut the edge off. That way if I were to change the hole PCD the cutoff would move accordingly.

Edited By JasonB on 08/05/2023 07:34:50

Doing it another way round where the distance to the cut edge is known and placing the first stud hole on that edge.

Nigel, I've said several times - if you get stuck contact me/Alibre for help. I'll either look at you files or do another screen share.

Rather than moan that 'x can't be done', instead maybe ask 'how can I do x?' or 'is it possible to do x?'

If you want to bring in geometry from a DXF/DWG, yes it opens in the Drawing workspace - from there you can copy/paste into 2D sketch of a part. The process is not complex, but you need to be aware of the steps. The basics are in the Help

There is a also a more detailed video (but I know you don't like videos).

If the engine block is already modelled, it can be placed in an assembly, then a new part created in the assembly for a cylinder cover. Edges and hole locations can be transferred from block to cover.

Maybe a bit advanced for Nigel until more experience is built up, but all readily doable in Atom3D.

That's right; those cylinder covers aren't "that simple"!

I think Nigel is trying to run before he has learned to walk. In CAD, as with almost everything else in life that's not bleeding obvious. you must grasp the basics before moving on. Confidence is good, over-confidence is bad.

"Blindly following an exercise" isn't good enough. Try doing the same exercise, but stop after each step and consider its purpose, asking 'what did that do?", and, "why is it necessary?" Don't jump to conclusions: if either question can't be answered, ask. David Jupp's offer is pure gold, and the forum's Alibre users know their stuff too.

Finally, that steam cover isn't a 'nightmare in CAD'. A trained operator can model one by applying a few few basic tools. But he has to be trained, and the hard part is learning what the basic steps are and how to apply them. Advanced CAD models are high risk if built without a reasonable grasp of the basics, and the software behaving oddly is a symptom of earlier operator mistakes. I crashed Solid Edge last week!

Dave

That cover is two concentric circles, a construction line, a 'solid' line and a point all completely constrained:

That's hardly complicated, is it? The geometry is fixed, so the actual dimensions are largely irrelevant. Although I would have modelled the cover in place at the top of the cylinder, using projected edges and known dimensions which is even easier.

Then it's an extrude for the cover and another for the recess. Use the hole tool centred on the point and a countersunk/counterbored/stepped is easy. Pattern that as required around the part's axis. Use the 'solid' line to cut off the corner. Finish with fillets/chamfers as required. In brass:

I've no proper drawings for any of this project; just a few ancient publicity photographs and one or two leading dimensions like the wheelbase and cylinder size. I made from these, some scrappy manual and TurboCAD drawings for various parts. Most of what's on the real thing is determined by measuring the pictures and parts I've already made without knowing what problems they will give, sometimes literally years, in the future.

I've reached a point I really need get things down on paper - manually or by CAD - before wasting yet more metal, electricity and hours on endless re-working.

'

Jason's model is what I was trying to achieve.

The cylinder covers looked simple, similar to an inconsequential Alibre exercise I had already created, a disc with a circle of holes. They proved so difficult, they showed I cannot draw the other parts or their assemblies.

I planned to draw the outer circle, then the holes, Trim the outline back to a line, then trim that line to form the edge; Extrude the combination, then make the register and recess.

Easier than the tutorials, using elements from them. Why should that fail?

The first screw hole was "undefined", Alibre told me, so useless. I could not draw the straight line where it should be; usually, no line at all. I have no idea why!

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Why:

A tiny, crossed-through circle next to the cursor? The Manual shows only a plain circle when the Circle tool is selected.

Objects permanently "defined" by size or location but not both (coloured orange), so useless?

The dimensions all lying on the axis, an illegible mess?

Some dimensions impossible to make? The flag said "parametric", but what was? What does it mean? The Manual does not explain it.

The few lines I managed to draw were all locked to the origin and axis?

More often, I could not draw any line at all? I can draw with any certainty, only concentric cylinders around the origin.

'

The Manual assumes you can't go wrong and it will always work. It does not explain where and why you can go wrong, and how to avoid doing so.

The trial licence has only a week to run and despite a promising start, buying the licence is becoming now an expensive gamble.

Thank you for the offer, David, but I can't keep troubling Mintronics every time I try to use Alibre by asking such totally basic questions.

'

No, I haven't tried to model the cylinder block, all circles and rectangles all at right-angles or parallel to each other. I have drawn it orthogonally in TurboCAD but though it's obviously easy for the experienced to draw it in 3D in Alibre, I doubt I could.

Nigel,

If you won't accept help when you are stuck, you won't learn.

All dimensions lying on an axis isn't at all clear - if you provide the part file, I'll be able to see what you are referring to. Alibre has a Help Desk team, and local resellers also provide support exactly because people need help to varying degrees.

If you won't accept help, then I don't think it's fair of you to post such negative comments about the software.

Keep sketches simple - I strongly advise against having the cover outline and the holes in a common sketch. I'll send you a file with my own approach where you'll see I use multiple features, each with a very simple sketch. See image below - this approach keeps each step simple, and makes it much easier to edit a step (or even delete and start again) without throwing away all the stuff that did work.

Extending your trial licence can be considered, but only if you accept help.

David, my gut feeling about the dimensions "all laying on the axis" is simply down to Nigel just leaving the mouse where it is after clicking the second of the two items being dimensioned.

I've done it here as I thing he is doing it, then repositioned them and then after removing the dimensions done it by positioning my mouse where I want the dimension befor entering it.

Something that you could have spotted in an instant if connected to his machine

Jason, Thx.

Nigel - dimensions appear where you place them.

• Click item to dimension
• (if appropriate click other item to dimension)
• Move cursor to position dimension - click to fix position
• Enter intended dimension value

You can click/drag dimensions later to re-position.

Edited By David Jupp on 08/05/2023 14:34:33

Have just got the answer on this - unfortunately the View Cube (a 3rd party provided component) created a few issues with other tools in 2D sketch mode, so the decision was taken to disable it.

Jason, David -

Thank you for that tip about dimensions.

I'll open one of those drawings and try it.... It's the most basic of those cover drawings, just the outline circle and the first bolt hole.

'

Sketch mode on, Correct plane (XY) on. Cleared the Undo buffer by stepping back until the arrow turned grey.

Select tool highlighted (blue background) but I can't select either circle. Clicking on them merely raises that summary tool-bar.

The Dimension tool is OFF (pale grey).

The Definition indicator says both circles are UN-defined in both magnitude and position. The main one is concentric with the displayed axis though.

Can I dimension the circles? NO.

Right, can I draw a line, anywhere? NO: Select 'Line', click somewhere on the image, nothing.

Click on the axis though, and I can draw a line apparently at any angle but always starting at the origin. The cursor has that little crossed-out circle stuck to it - don;t know what that tells me.

I drew two lines of set lengths, one along the X-axis, the other Y (by entering 90º ). The X-axis line is defined by magnitude but not position (yet it's on the axis and origin?); the Y-line is fully defined.

Can I draw a line from their end nodes?

Yes from the Y-one.

Oh - the X-one is now shown as fully-"defined" (how did that happen?) and I can now draw a line from it.

Something turned on Dimensions too.

I've now a peculiar thing with two pairs of +ve and -ve going, straight lines of equal lengths, like steps, and a line joining the extreme ends, through the origin. I can't dimension that though, because it hits that "parametric" thing I know nothing about.

I tried dragging the dimensions left on from drawing the first two lines, but could not move them. I only made them collapse onto the axis. Then found by selecting the Dimension tool again they jumped back to their original places.

Dimension the circles? No. They are still Undefined.

Let's try re-drawing the main circle....

I should have really deleted the first but since I can't select it had to leave it. I've now a fully-defined new circle but the dimension I tried to place did not respond to my attempts to place it neatly. All I did was scrunch it up on the axis, and I could not click and drag any of the dimensions anywhere.

.

Finally, I tried to close it, which opens the Analyse menu. This revealed 27 faults, all but one being described as incurable! (Except by Nature giving the operator an IQ of 140 and learning ability to match.......)

'

Then you all wonder why I find the thing so difficult and frustrating: I can't make the simplest drawings..

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I will re-iterate...

..... I do not denigrate the software!

In fact of the three makes of CAD I have tried, Alibre seems the easiest to learn, at least to a fairly useful level even if I could never construct a 3D image of something like that engine on the publisher's own web-site. Or of my steam-lorry.

It's me, not it, that has the problems. Perhaps I am physically unable to learn such software; just as I was unable to learn Mathematics or French, to play the piano, or be any good at sports and games. That is me, by Nature, not the programmers' fault, not some mysterious artefact of CAD!

I do not refuse help. If that were the case I would not ask on here, let alone have accepted that offered tutorial last week. I don't though, want to impose on the publishers by asking questions that are just so basic as how to draw a line in the right place in one go every time.

Edited By Nigel Graham 2 on 08/05/2023 16:06:45

Nigel - you don't actually appear to ASK here, you just give vague descriptions of your activities and the outcomes. Not clear enough to really work out what problem you are hitting. Not even any screenshots of any of the problems.

Hopefully showing exactly what went wrong would lead either to you learning, or to Alibre being made aware of an unappreciated pitfall in use of the software.

PLEASE send me for example your file with 27 errors in a sketch (tell me which sketch, to save time). There isn't an 'incurable' output - the 'heal' button can only address certain error types, for most the user has to resolve them. 27 faults suggests a 'busy' sketch. This is another reason why I strongly recommend the use of simple sketches - much easier to diagnose, and less work wasted if you do have to abandon a sketch.

I don't see any big difference between asking for help here or directly from Alibre, or via the Alibre user forum.

You are trying to select items in a new sketch before you have added any and are just clicking away at the underlying previous sketch

You need to do what David says and give him access to the files and screen shorts or even just a photo of the screen if you can't do a screen shot.

Edited By JasonB on 08/05/2023 16:54:54

Edited By JasonB on 08/05/2023 18:11:18

He's not even getting to draw/sketch/edit mode, just clicking about randomly with select

I feel he is getting to sketch mode, can't be bothered to do a video to show it but I can replicate not being able to select what he thinks is in a sketch.

Also sounds like Ordinate dimensions has been clicked at some time hence the odd numbers. Again just problems with that odd mouse and not being used to using the new one.

I doubt it is coming up saying Parametric. The two options you get are Parameter and Driven when dimensioning a sketch

Edited By JasonB on 08/05/2023 17:13:43

Yes he's into sketch but only using select for everything

I've reached a point I really need get things down on paper - manually or by CAD - before wasting yet more metal, electricity and hours on endless re-working.

Nigel you're doing exactly the right thing by going for CAD in this situation btw

Edited By Ady1 on 08/05/2023 17:50:19

Nigel,

To edit an existing sketch, locate it in the Design Explorer (left hand side of screen), right click on it and select 'Edit' from the options in the context menu.

You should then be able to modify the sketch figures or dimensions.

Using the 'Activate 2D Sketch' button will open a NEW sketch. You can have multiple different sketches on any plane or flat face.