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Sweep problem - can't select sketch

18 REPLIES 18
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Message 1 of 19
mbus0013
4920 Views, 18 Replies

Sweep problem - can't select sketch

I am trying to make a model of a bicycle wheel. I created a 3d sketch using a line and an arc for the spoke, did a 2-D sketch of a circle on the hub where the spoke should end and i'm trying to sweep this circle along the required path.

The problem is that when I click sweep and try to select the cicle I sketch I can't!

I did use sweep before for other parts without such problem. I also tried creating a plane using the centre of the circle an the 3d line to ensure that the sketch is perpendicular to the line but still the same problem - what am I doing wrong?

 

If anyone has any idea on how to do the spokes using any other method please do tell!

18 REPLIES 18
Message 2 of 19
bcrowell
in reply to: mbus0013

Are you using INV2012?  I'm on 2011 and couldn't open the file.

 

Something you may want to do is include your system information in your signature- some users will fuss at you if they try to help and that information isn't there.  Just an FYI.

 

 

INV Professional 2017 (Build: 142, Release: 2017RTM), Windows 10 Professional (64-bit), Intel Xeon E5-1620 3.5GHz CPU, 32GB RAM, NVIDIA Quadro K2200, Vault Basic 2017
Message 3 of 19
JDMather
in reply to: mbus0013

First thing I noticed is that your Sketch1 is not constrained.

It would make logical sense for the end of the horizontal line to be a the origin so that your axis of revolution is about the y-axis.

I recommend you read this document.

http://home.pct.edu/~jmather/skillsusa%20university.pdf

 

You should have multiple solid bodies in the file.

For example if you edit Revolution2 you should have New Solid selected.

 

The bend in your spoke is too small (among other problems with the path).

 

The holes in the rim are incorrect.

 

Holes.png


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Message 4 of 19
mbus0013
in reply to: mbus0013

Thank you for your reply.

However my problem is still the same - I can't sweep the shape (spokes) I want. Any help with that?

Message 5 of 19
JDMather
in reply to: mbus0013


@mbus0013 wrote:

 Any help with that?


I would not be able to help until you fix the foundation problems - maybe someone else will jump in here.

Once you fix the foundation problems the solution to your immediate problem is rather trivial.


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Message 6 of 19
trumpy81
in reply to: JDMather

The above comments about your sketches being unconstrained are true. Go back to Sketch 1 and make sure all the geometry is fully constrained.

 

Next point, you cannot use a 2D sketch and a 3D sketch for the sweep command (as far as I know anyhow). You need 2 x 2D sketches for that.

 

Another point is that bicycle spokes are straight. If you had a curved spoke then you would have a serious problem with your wheel.

Regards
Andy M
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Message 7 of 19
rhasell
in reply to: trumpy81

Hi besides the issues mentioned earlier, the problem with the sweep is the radius of the 3d sketch at the bend of the spoke.

 

The spoke intersects with it's self. There is also an issue with the termination, but thats for you to look at, Use "New solid" to bypass this.

 

 

Reg
2024.2
Please Accept as a solution / Kudos
Message 8 of 19
rhasell
in reply to: rhasell

other image did not attach.

Reg
2024.2
Please Accept as a solution / Kudos
Message 9 of 19
trumpy81
in reply to: rhasell


@rhasell wrote:

The spoke intersects with it's self. There is also an issue with the termination, but thats for you to look at, Use "New solid" to bypass this.


rhasell, could you clarify how the spoke intersects with it's self please. I ask because, recently, I have had some errors reporting self intersecting lines etc... but I could not see any evidence anywhere that a line or other geometry was intersecting itself.

 

I guess this could be just my understanding of the meaning behind it, but I'm curious to know what it does mean.

 

TIA

Regards
Andy M
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Autodesk Inventor 2013 Pro SP1.1, Win7 Pro - 64Bit - SP1, Intel i7 960 @ 3.333 GHz
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Message 10 of 19
rhasell
in reply to: mbus0013

Hi, I am replying from my mobile, so please be patient.

The sweep path might look good, but the resultant solid defies the rules. When modeling a part remember that it has to be manufactured. Eg, the spoke will never be able to be manufactured using the radius of.0.6mm for a 2.5mm diameter wire.

Without seeing your other parts it is hard to comment.

I try and use logic and manufacturing experience when designing. Granted molds/casting/machining require a different set of skills and modelling tricks.

I will respond again once I am in front of a computer if no-one else has chipped in.
Reg.
Reg
2024.2
Please Accept as a solution / Kudos
Message 11 of 19
trumpy81
in reply to: rhasell

Reg, thanks for the reply.

 

FYI, I'm not the OP, I'm simply interested in how things are labelled as being self intersecting when I can see no evidence of it in Inventor.

 

In the example part, the geometry to my mind does not show any self intersecting even in the solid state. Granted, the part as drawn could not be manufactured easily, unless it were machined from solid, which would be of no advantage at all and would certainly not be cost effective, but it is possible!

 

So the question remains where and how does this geometry self intersect, according to Inventor at least?

 

Is Inventor seeing the 0.6mm bend radius as being impossible and then declaring self intersection or is there something else that I'm not seeing/understanding?

 

I too, try to follow standard manufacturing processes when designing my own parts, but every now and then I strike this error and I can not understand why. I'm well aware of minimum bend radius, modulus of elasticity etc... for given materials so it would seem unlikely that I would break those rules, yet Inventor tells me otherwise. Of course, I have made some pretty obvious errors, but a lot of the time they are not so obvious and they're the ones that bug me ... lol

Regards
Andy M
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Autodesk Inventor 2013 Pro SP1.1, Win7 Pro - 64Bit - SP1, Intel i7 960 @ 3.333 GHz
Asus X58 Sabertooth, Corsair 12Gig DDR3, AMD Radeon HD6970, Samsung 830 Series 256G SSD, 2x 3TB Seagate, 2x 2TB Hitachi,
1x 1TB Samsung, 4 x 2TB Seagate in Netgear ReadyNAS NV+, Dual Asus VE278Q Monitors
Message 12 of 19
rhasell
in reply to: mbus0013

Have to agree on Inventor not doing what I ask it to do, or a part breaking a few months down the line, but nine times out of ten, its my fault. Occasionally I dump it and try another route with the same/better results.

This forum is great, I have learnt so much from it, thanks everyo, though I still have unanswered questions with the forum and Autodesk.
Reg.
Reg
2024.2
Please Accept as a solution / Kudos
Message 13 of 19
JDMather
in reply to: trumpy81


@trumpy81 wrote:

Next point, you cannot use a 2D sketch and a 3D sketch for the sweep command (as far as I know anyhow).


 

Of course you can.  You might go through the tutorials in my signature (Knot comes to mind).

 


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Message 14 of 19
JDMather
in reply to: trumpy81


@trumpy81 wrote:

 I have had some errors reporting self intersecting lines etc... but I could not see any evidence anywhere that a line or other geometry was intersecting itself. 

Attach file here that exhibits this behavior.


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Message 15 of 19
mbus0013
in reply to: trumpy81

I have edited the holes on the rim, thanks for pointing that out

I have increased the radius of the curve

But no matter what circle I sketch, when I click sweep and try to select is as profile it just won't select it! I can't understand why

Message 16 of 19
JDMather
in reply to: mbus0013


@mbus0013 wrote:

I have edited the holes on the rim, thanks for pointing that out

I have increased the radius of the curve

But no matter what circle I sketch, when I click sweep and try to select is as profile it just won't select it! I can't understand why


Attach the new file here.


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Message 17 of 19
mbus0013
in reply to: JDMather

In the end I started the wheel from scratch, used a similar method and had no problems with the sweep.

I still don't know why I kept getting this problem but at least I don't have to solve it anymore.

Thanks everyone for trying to help.

Message 18 of 19
JDMather
in reply to: mbus0013


@mbus0013 wrote:

I still don't know why I kept getting this problem but at least I don't have to solve it anymore.


Your sweep would have created a self-intersecting body.  It could have been fixed.


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Message 19 of 19
glenn-chun
in reply to: mbus0013

Back to the original question using your wheel 24.ipt, the reason why you couldn't easily select the circle in Sketch13 as a sweep profile is that there are too many visible sketches that can be a sweep profile.  Especially, the huge circles in Sketch6 get highlighted first as a sweep profile.  If you turn off the visibility of Sketch6, the small circle in Sketch13 can be easily selected.  Otherwise, you could zoom in the small circle and right-click > Select Other > 2. Profile Body.

 

HTH,

Glenn



Glenn Chun
Sr. Principal Engineer

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