Major Problems with Sweep in Inventor 2014

[ccoomes]

The company I work for manufactures bend Wire Parts in different shapes and sizes.

To create this we use the Sweep Command to sweep a profile around a 3D.  The 3D sketch is created from Points (So we can export the XYZ Coordinates into our machines) the are controlled by Numerous 2D Sketches.  The points are joined together using the line command (Within the 3D sketch) with a radius between each line.

In Inventor 2010, any changes made to the Sweep, or when creating a new sweep when you clicked the profile (In the Sweep Dialog Box) it followed the COMPLETE Profile or updated the profile to the new changes.

However, in Inventor 2014 when you click the profile if highlights the Complete profile, but when you click OK it will ONLY select the First Length of the 3D Sketch.  It gives you an error stating that the path does not intersect the profile (Which is DOES) and do you want to continue.  If you select yes, it then gives you another error which you click accept.  The Sweep is then only attached to the FIRST line in the 3D sketch.

To get the full profile selected, you then have to edit the Sweep just created and MANUALLY click each line and Radius of the 3D sketch to get the sweep to follow full profile.

This is the same when you try to modify a part created in Inventor 2010, it will NOT select the full path, just the first line.  You will then need to manually edit the sweep and select each line a radius of the 3D Sketch.

The Sweep command worked perfectly in Inventor 2010, and we now have something that does not work correctly at all in Inventor 2014...

Can someone from Autodesk please confirm why this has been changed, and if it going to be resolved in the Service Pack 1 for Inventor 2014?

[Martin.Tomko]

Hi,

could you, please, provide us simple dataset created on Inventor 2014 with sweep profile and sweep path ? If you could attach also short video with detailed steps including error dialog, it would be great. I tried it on my own dataset ( work points in 3D sketch connected by lines with a radius between each line), but I don´t see this problem. Many thanks!

Regards,

Martin

[ccoomes]

Hi Martin,

Please find attached a zip file containing the ipt File of the part and the Excel file that is linked to the Part.

The Sweep has been deleted the from the Part and just left the 3D Sketch and the 2D Sketches Required.

I tried to add a new sweep using the 3D Sketch and Profile and it gets the same error as I have listed in my first post.

This happens on 2 Machines in our office, and both are running Inventor 2014 with Updates 1 & 2 Installed.

Can you please offer a solution to this as we never had any problems with this in Inventor 2010..

Many Thanks.

[Martin.Tomko]

Hi,

thank you for provided dataset!  I will log a defect into the our internal database, thank you for reporting this issue. While it will be fixed by developer I have work around for you. 

So he are the steps:

1. Invoke "Sweep" command

2. Select sweep profile ( will be selected automatically in this case)

3. Right mouse button (RMB) click to the sweep path

4. Click to the "Select Other" in the context menu and choose "Curve"  from dropdown menu

5. Now select the rest of the sweep path by LMB ( left mouse button) clicking and press "Ok"

result: Sweep feature should be created.

I hope it helps.

Regards,

Martin

[ccoomes]

Hi,

Thank you for the quick 'Fix'.

Can you please tell me when it will be fully fixed so the sweep command works as it should?

Will it make it into Service Pack 1, if so when is service pack 1 due for release?

Many Thanks.

[Martin.Tomko]

Hi,

I don't know if it will be included into th SP1, it must be assessed by managment according to the priority.

Regards,

Martin

[JDMather]

I don't want to detract from the problem you found with r2014, but do you have any leeway with how those bends are made?  (see attached)

I am also working on a version that matches your original post.

[ccoomes]

Hi JDMathers,

I understand that there are lots of ways you can create what I posted, but please read my first post about using the 3D Sketch Points to Export the XYZ Corrdinates to allow our machines to manufacture the Parts.

The Sweep Feature worked Perfectly in Inventor 2010 and how the part is drawn was not my original question, but to highlight the fact that the Sweep Feature in Inventor 2014 was not working.

As the Sweep Feature is not Working in Inventor 2014 (It was in previous Versions (2008, 2009 & 2010)), can Autodesk please explain WHY it may not be corrected in Service Pack 1?  It is Fault in Software that was NOT previously present...

[ccoomes]

HI JDMAthers,

Sorry, your text to your post appeared while I was tying my response.

Unfortunuely, we are governed by what our Machines can bend and the tooling they use.  The Wire is Bent around Mandrells that are Certain Diameters to Suit the different Diameters in Wire.

The Part posted was for a Ø4.75 Wire Part Bent using a Ø5.00 Mandrell.

We also have to factor in bits like the what the Minimum straight shank needs to be for the part to be bent, who the part rotates to avoid the Bending Head and Table long with other issues...

Sometimes simple parts on the screen can be a nightmare to manfuacture on the machines...

Please feel free to ask if you would any assistance in drawing wire parts to make them easy to modify and control.

Many thanks in advance.

[JDMather]

I suspected that was the case.

I think I can still work up another simplified solution that returns the exact geometry you are after and solves your problem.

Let me work with it a bit longer and see what I can come up with.

But as you indicated - I don't see why this should have created a particular problem in 2014.  I think you might have discovered a bug (err, issue) with 2014.

[ccoomes]

Hi,

If you find a simple solution please let us know.

Some other things that must be considered when you create the part are:

The Points MUST be the intersection of the 2 Lines and with a Fillet between the 2 lines.

The Points MUST be in the Correct Sequence of the Path (First point is the Start and the Last point is the Finish)

In IV2010 you could NOT Mirror Complete Sketches (Hence the 2nd Sketch for the Front Raised Section)

In IV2010 you could Mirror 3D Work Points (I Think) BUT the Points had NO XYZ Coordinates and they did NOT appear in the correct sequence, it was a random sequence...

I have not had a chance to test if the last 2 points have changed in IV2014...

If I think of anything else that we have to follow I will add it.

To be honest, I sometimes draw parts in a complicated way, but this makes them easier to modify and control for different products, customers etc.

I can concurr that I have found a very BIG Bug in IV2014 and would now ask AutoDesk to confirm it will be fixed for Service Pack 1?

[johnsonshiue]

Hi! Many thanks for reporting this issue to us! Base on my priliminary analysis, it seems to have something to do with the two continuous bends. There is a degenerated segment (becoming a point) in the middle. For some reason, Inventor stops recognizing it as a valid path. I am able to reproduce the behavior on R2012 and later. The same path does work in R2011 or earlier. The new behavior is wrong. The Sweep should work in this case regardless.

Before a fix to the issue is available, you can consider using the workaround Martin has identified or you can use Arc command (instead of Bend leading to degenerated segment) to create the round. I am very sorry for the inconvience the behavior has introduced. I will work with the team to get this behavior corrected soon.

Thanks again!

[glenn-chun]

This is an Inventor defect introduced in Inventor 2012 as Johnson found out.  Martin logged this issue as 1505208.

Attached is a simpler model last saved in Inventor 2011.  The 3D sketch has a line between two bends:

This line degenerates to a point when the bend radius is changed to 15 mm and two bends meet each other:

Sweep can be created successfully in Inventor 2011:

Inventor 2012, however, doesn't think this is a valid path. So Inventor requests ASM to sweep the profile along the first path segment only:

Until the Inventor team fixes this defect, please use one of the following workarounds:

Workaround #1: Individually select the path segments (This is what Martin mentioned earlier).

Click the remaining segments, one at a time.

Workaround #2: Replace two bends with one arc.

Workaround #3: Sweep along a path with no degeneracy and then edit the path.

Edit the path to introduce some degeneracies.

Sweep will recompute successfully.

Glenn

ASM Development

[ccoomes]

Hi GlenChun,

Thank you for the suggestions on how to draw the parts, but please read ALL my posts.

We are governed by our Machines and cannot always have a complete curve between 2 lines, there may need to be a straight shank between 2 bends.

There are no options but the use the 'Workarounds'...

Dear Autodesk,

This is a fundamental fault in Inventor for 3 versions (2012, 2013 & 2014 and Numerous Service Packs & Updates for each version) for a Basic Feature.

This is really great customer support from Autodesk when you don't fix simple errors of a basic feature that worked in Inventor 2010 Perfectly.

All Autodesk seem interested in with the latest releases is making sure it can makes things look pretty.  Don't worry about their customers who bought the software for what it was design for, Engineering and Manufacture.....

Looks like I can expect it NOT to be fixed in Service Pack 1 if it has not been fixed in 3 Versions....

Thank you for all your posts and another satisfied Autodesk Customer off to speak to their reseller...

[ccoomes]

After a fair amount of testing, we can confirm that this issue has NOT been resolved with Inventor 2014 Service Pack 1.

My colleague and myself have had to use the 'quick fix' method (as posted in this topic) on numerous new parts created since IV2014 Service Pack 1 has been installed.

Similar parts worked perfectly in Inventor 2010 and previous versions of the Software.

Thank you to all who have posted with help, the work arounds and for different methods for creating the parts.

Thank you also to Autodesk for ensuring that long running Software faults (This worked fine in Inventor 2010 and has NOT since IV 2013) are fixed as a priority.