Irregular alignments

[doodah]

I've been following some tutorials and have got myself stable in some basic understanding and manipulation of the geometry, however all of the examples have nicely aligned parts, which is unfortunately different from my experimental real-world project.

In my head, I'd want to move a vertex by deforming the shape rather than moving an edge or face (moving the purple vertex to the red one in my screenshot).

You can see that the front (left side) is wider than the rear (right side), which, when rotating the two sides inwards equally has created a very small overlap in the front connecting piece and a gap in the rear piece. What's the common practice or technique for dealing with this?

 

[SSIMMONS]

In my personal opinion, this is more or a manufacturing limitation question. In a lot of circumstances you would fill the gap with weld so the way you have it would be fine because the stock, sheet, etc. being used will have a square face and it is often not worth paying for special machining of the part to fit flush like you are saying. I think most people approach these in different ways depending on the type of manufacturing they are used to and the limitations they have to live with. Now, that being said, you can either break it back to flush right before the right side seen above in your snip or you can add material and slice it off with a hole block to make it pretty and clean looking. The easiest would be to modify the cross-section of the block you have on the right side that is bridging the two halves.  Just depends what you are doing with it really. Very vague and back and forth answer, but just my 2 cents worth.

 

- Spencer

Edited June 29, 2021 by SSIMMONS
Additional Information

[doodah]

Thanks Spencer - Actually that does answer the question and your insight into weld joints is really interesting.

Perhaps I should have explained that my whole reason for getting into IronCAD was for 3D printing as the interface seems so much easier to get to grips with from other CAD / modelling software I've experimented with. The part boundaries need to be pretty exact, and your video explained precisely how to do this so thanks for taking the time to record that.

My issue is now that I can't edit the sketch in the plane I want. Your video actually showed you had the same problem and re-orientated the block to get the sketch plane right, so that suddenly clicked that the orientation of the part is linked to the edit cross-section orientation... My new issue is that I shaped the joining block with it's cross section on the x-y plane, so that it has a specific shape in-situ. I need to edit the cross section in the y-z plane to mimic what you did in your video but can't rotate the part to do this without messing stuff up.

I've tried searching for the answer, however I can't seem to find this particular scenario.

I guess what I'm asking is; can you edit multiple plane cross sections for the same part?

[Mike Hatch]

Instead of manipulating a block into the space I'd have directly drawn a 2D sketch and extruded it. 

It gets you to the same place a bit quicker, just a different way of skinning that cat.

You could apply a draft to fill it in.

[Jonas@Solidmakarna]

As Mike says, creating a new Sketch based model is a fast way to go!

The shapes (pre-made features) in the Starter (and Shapes) catalogs are symmetrical and "simple" in many ways, but they can all be manipulated. If you have dropped a Block shape, you can edit the 2D Sketch (also called Cross-Section) of that shape and make any kind of change to the curves there.

But there are other options too! Here are two simple ways with the standard tools;

Chamfer feature (Distance/Distance):

Make sure the part you add the Chamfer to (the Blue Part in this case below) is larger than (or "crosses over") the other part and matches at least in one corner (top left, in this case below).

Chamfer from the top right corner and use the Chamfer feature handles on each side to snap (while holding down the [Shift] key) to the values as needed (or just type them if you know the values):

Sketch based edit:

How to make the curve fit exactly as how you want it, that depends on your preferences and the shapes. I think dragging a knee point could work in this case.
You could also remove the curve and Project a new curve from the edge of the other part. Then trim/extend to make an "unbroken" single contour (of the blue part below).

The upper curve will now "match" the other part edge.

Finish the Sketch.

 

[Mike Hatch]

You can also add an HBlock and orientate it to the second part, a bit more brutal but its quick.

Edited June 30, 2021 by Mike Hatch

[SSIMMONS]

I am not sure exactly what you are trying to do in the other plane, but maybe this will help. I also modeled the piece in two different ways just so you have options, There are many many ways to do this, but it really just comes down to personal preference and workflow setup. I have 12 keys on my mouse so I hardly use a keyboard for the most part (really only when I input numbers, though the mouse can do that also) and this creates an extremely rapid modeling setup, but I will say it takes a toll on the old wrist. When it shows the number keys being pressed in my videos, it is actually just a mouse. 

 

- Spencer

[doodah]

Sorry for the delay in responding all. It's been a busy couple of days in the real world. So I really appreciate all of the suggestions, and I think I'm slowly getting to grips with the basic sketch manipulation. I now appreciate the split function and how it's more-or-less the same for operations like this.

So, I realise @SSIMMONS I didn't do a great job of explaining what I meant by my need to edit the same volume on two sketch planes. Even if that's possible (or not), I'm willing to bet at this stage you guys have a better way of doing what I'm trying to get to. (Again, really appreciate your guessing at what I was trying to explain with those vids).

I'll try and explain things a bit clearer this time - with images!

Now I have the joining part added as I was trying to do originally. The face I've highlighted is a trapezoid and meshes with the two angled pieces either side perfectly. 

However, the "other plane" I mentioned was the side profile of the part, where I want it to match the curve of the side parts, like this:

I've played around with some multiple point chamfer and blend edges, but I can't get a good result.

If I could edit this side as a cross section, then I'm sure I would b e able to add points and match it up perfectly. So this is my current issue.

 

[ASPEER]

you can make a hole extrude to remove the section you dont want, you could even make it follow a curve so that the two blends are continuous, or perhaps a better option would be using a sweep with the side profile you want and have it sweep from face to face.

Edited July 1, 2021 by ASPEER
add images

[SSIMMONS]

16 hours ago, doodah said:

Sorry for the delay in responding all. It's been a busy couple of days in the real world. So I really appreciate all of the suggestions, and I think I'm slowly getting to grips with the basic sketch manipulation. I now appreciate the split function and how it's more-or-less the same for operations like this.

So, I realise @SSIMMONS I didn't do a great job of explaining what I meant by my need to edit the same volume on two sketch planes. Even if that's possible (or not), I'm willing to bet at this stage you guys have a better way of doing what I'm trying to get to. (Again, really appreciate your guessing at what I was trying to explain with those vids).

I'll try and explain things a bit clearer this time - with images!

Now I have the joining part added as I was trying to do originally. The face I've highlighted is a trapezoid and meshes with the two angled pieces either side perfectly. 

However, the "other plane" I mentioned was the side profile of the part, where I want it to match the curve of the side parts, like this:

I've played around with some multiple point chamfer and blend edges, but I can't get a good result.

If I could edit this side as a cross section, then I'm sure I would b e able to add points and match it up perfectly. So this is my current issue.

 

Anytime you need to do something like this and the cross section is not oriented with the screen, you can use a hole block on that part and edit the cross-section of the hole block itself. I will attach a video showing the process of cross-section edits of hole blocks, but it is essentially the same as any other. The notable difference being you are removing instead of adding material. Use projections and you can match the other profile exactly. Just be careful because since your parts are not perfectly aligned due to the dill piece being a trapezoid, the projection can be relative to a different plane sometimes and not do what you expect, but you will work this out naturally in time. Good Luck!

 

-Spencer

 

Edited July 2, 2021 by SSIMMONS