Inventor General Discussion

Inventor General Discussion

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Member
jdexter
Posts: 5
Registered: ‎01-12-2013
Message 1 of 11 (1,214 Views)

Struggling with Sweep command

1214 Views, 10 Replies
01-12-2013 12:09 PM

When I try to sweep a circle along the curve in the attached file, it only goes round the first curve and I can't find a way to persuade it to go further. I created the curve by drawing parallel straight lines and joining them with circles before trimming. Automatic dimensioning does not show any errors. I am trying to end up with a representation of a 'serpent' musical instrument which is a tapered tube - the end circles in the sketch being the relevant dimensions of each end - a taper of about -2.064 degrees from the wider end. I cannot find anything amongst the tutorials or forums that seem to be relevant. I am somewhat new to Inventor though quite experienced in Autocad. Help would be much appreciated - thanks.

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blair
Posts: 4,082
Registered: ‎11-13-2006
Message 2 of 11 (1,209 Views)

Re: Struggling with Sweep command

01-12-2013 01:04 PM in reply to: jdexter

1.) Looking at your file, you are starting with a small circle profile and hoping to end with a larger circle profile. This can't be done with a Sweep, as it only uses a single profile for the shape and then a path. You should be looking at the Loft command.

 

2.) You have a sketch problem where your path stops at the end of your 244.509 radius to the 57.6 line segment. If you zoom you will see a problem with the end of the arc and start of the line. The arc attaches to the line not at the beginning of the line, but at a distance 2 units from the line end.

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SpacePilot Pro 3.17.7, 6.17., 4.11
Member
jdexter
Posts: 5
Registered: ‎01-12-2013
Message 3 of 11 (1,202 Views)

Re: Struggling with Sweep command

01-12-2013 01:13 PM in reply to: blair

Thanks Blair, I'll look at that.. when I was trying the sweep command I was only using the larger circle and setting a value for angle in the sweep box. I didn't realise the loft command would follow a path also - I'll have a look at that also.

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JDMather
Posts: 26,612
Registered: ‎04-20-2006
Message 4 of 11 (1,200 Views)

Re: Struggling with Sweep command

01-12-2013 01:16 PM in reply to: jdexter

jdexter wrote:

Automatic dimensioning does not show any errors.


 

I recommend that you forget that you ever saw autodimension.

Your sketch dimensions should look like something you would send out to the shop floor on a drawing.

Send that mess out - and you will lose all credibility.


Edit your Sketch1.
Right click and select Show All Constraints.
You should have Tangent constraints between each entity in your path.

and as suggested - use Loft with the centerline option.
Please mark this response as "Accept as Solution" if it answers your question.
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Member
jdexter
Posts: 5
Registered: ‎01-12-2013
Message 5 of 11 (1,190 Views)

Re: Struggling with Sweep command

01-12-2013 03:28 PM in reply to: JDMather

I think I have cleaned up the sketch pretty well but, when I try the Loft command, I am getting an error saying that the 'curve is not smooth'. I can't see any command which would help with this and I don't really want to change the shape of the curve as it is a measured drawing from an actual instrument. Is there any solution to this? thanks.

(cleaned up file attached)

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blair
Posts: 4,082
Registered: ‎11-13-2006
Message 6 of 11 (1,167 Views)

Re: Struggling with Sweep command

01-13-2013 01:30 AM in reply to: jdexter

You primary sketch is not fully constrained and can be moved around. I suspect this is your primary problem. Start the sketch from the Origin Point which will anchor it. I would start the end with the small end at the origin point and then fully dimension the S-shape part. Then create your small end profile on one of the Origin Planes at the Origin. Then create a work plane at the other end (large end), Inventor will create a work-plane perpendicular to this end by default. Start your sketch on this work plane, project the end of the profile line on this sketch to constrain the large end profile, then create your end profile. This really shouldn't take more than 5 minutes to do, most of the time will be spent placing the dimensions on the profile path (first sketch).Image.jpg

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IV2015 up2 PDSU / Sim Mech 2015 /
Win7-64
EVGA X79 - Classified, iCore7 3930k 32Gb Quad-Channel
950Gb (2 x 500Gb Sata III SSD RAID0 Adaptec 6805E Controller)
Nvidia GTX-690 Classified - 335.23
SpacePilot Pro 3.17.7, 6.17., 4.11
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blair
Posts: 4,082
Registered: ‎11-13-2006
Message 7 of 11 (1,164 Views)

Re: Struggling with Sweep command

01-13-2013 01:41 AM in reply to: jdexter

Like this, I just dragged your sketch so the small end is at the Origin point and constrained to it. This could be cleaned up even more. You didn't have the large end of the primary sketch properly constrained/dimensioned. 

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IV2015 up2 PDSU / Sim Mech 2015 /
Win7-64
EVGA X79 - Classified, iCore7 3930k 32Gb Quad-Channel
950Gb (2 x 500Gb Sata III SSD RAID0 Adaptec 6805E Controller)
Nvidia GTX-690 Classified - 335.23
SpacePilot Pro 3.17.7, 6.17., 4.11
Employee
GlennChun
Posts: 115
Registered: ‎06-10-2004
Message 8 of 11 (1,155 Views)

Re: Struggling with Sweep command

01-13-2013 02:04 AM in reply to: jdexter

Hi jdexter,

 

The path sketch in your centreline-1.ipt is better than that in centreline.ipt, but it's still not tangent-continuous.  Edit the sketch and hit F8 to show all constraints.  Four tangent constraints are missing as indicated below.

 

not_tangent_continuous.png

 

Once you make the path tangent-continuous (See centreline-gc-tangent.ipt), either sweep or loft will be successful.  It is important to make the path tangent-continuous for tapered sweep and centerline loft.  As many other users suggested, always make your sketches fully constrained.

 

In ASM (the geometric modeling engine for Inventor, AutoCAD, etc.), sweep can take either taper angle or taper distance.  In your model, you want the radius of the circular profile to change from 56 mm to 10.5 mm, so the taper distance is -45.5 mm.  Inventor can take a taper angle, but not taper distance.  Here's a formula that computes the taper angle when the taper distance and path length are given:

 

taperAngle = arctan( taperDistance / pathLength )

 

You can use the Measure Loop tool to obtain the path length.  In centreline-gc-tangent.ipt, the path length is 2149.09641 mm.  The taper angle is then acrtan(-45.5 mm / 2149.09641 mm) = -1.2128672 deg.  If you sweep the large circle using this taper angle, the diameter of the end cap face will be the desired 21 mm.  See centreline-gc-sweep.ipt

 

sweep.png

 

For the lateral faces, sweep creates five spline faces and four cones shown in red above.  Analytical geometry such as cone, cylinder, and torus is much lighter and faster than spline surface.

 

Loft creates a single lateral face which is a long spline face as shown below.  See centreline-gc-loft.ipt

 

loft.png

 

Hope this helps,

 

Glenn

ASM Development

Autodesk T-Splines Component Development
Member
jdexter
Posts: 5
Registered: ‎01-12-2013
Message 9 of 11 (1,143 Views)

Re: Struggling with Sweep command

01-13-2013 02:58 AM in reply to: GlennChun

Thanks everyone - I have now managed to loft the shape myself following your instructions. I do have a couple more queries while I'm working on this file and learning...

The size of the smaller end circle in my file was wrong - I had used the radius instead of the diameter which should be 42mm. I would now like to draw the internal bore of the pipe which, from the larger open end, mostly has a wall thickness of 6mm but narrows to 23mm diameter at a point 75mm from the small end from where it goes as a 23mm parallel bore to the small end. I assume I can split the centreline path at a point maybe 12mm from the small end and use the Shell command to do the larger part of the bore ( although I'm not sure whether I would then have to punch a hole through the large end with the Hole command or not), however, I am not sure how to deal with the taper from whatever the shell internal diameter at 120mm is, to the 23mm at 75mm. Does Inventor have a 'Difference' command like Autocad or some other way to subtract one 3D shape from another - I haven't found one yet...  Thanks for your patience..

Member
jdexter
Posts: 5
Registered: ‎01-12-2013
Message 10 of 11 (1,141 Views)

Re: Struggling with Sweep command

01-13-2013 03:00 AM in reply to: jdexter

Oh, I forgot, how do you measure the total length of the centreline and can I then scale it? I need to finish up with a total path length of 1942mm. Thanks..

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