Sheet metal loft woes

[HDEAR]

A good proportion of our products consist of sheet metal transitions; square to round symetrical, square to round offset centre, round to round symetrical, and round to round offset centres.

 

Having spent the weekend going through IC lessons, I can't for the life of me get the lofted sheetmetal transistions and their developments ( unfold ) working properly. I'm screwing up, but do not know where. I bet it's a simple step I'm getting wrong or missing.

 

Attached;

 

1) Transition of what I expect it to look like with all development folds where you'd expect them ( SWX lesson )

2) The resultant development ( fold out )

3) Using IC Loft wizard - various steps and the results ( lousy unfold out shape and development fold lines)

4) Steps using sketch, trimming a gap, copying to another plane, resize, loft and trial unfold - ends up just a line!

 

The attached files should be in sequence of my explanation above

 

HELP!

Edited August 3, 2014 by HDEAR

[dleczynski]

Movie How Loft Edited August 3, 2014 by dleczynski

[HDEAR]

Movie How Loft

38374[/snapback]

Thank you. I followed your instruction exactly.

 

Unfortunately, when it came to the unfold, all I got was the line as shown below.

 

So something's happening when I hit the unfold button. It maybe a setting I have wrong or one simple step during the loft build process, however I have now followed several sets of instructions and got the same 1 line result when pressing unfold.

Edited August 4, 2014 by HDEAR

[jolizon590016]

I have to file this to bug reports and hopefully a resolution can be made. I am experiencing what Harley has been doing and I am coming up with same results also with Dariusz video. I have tried it with my other notebook running 2014 also with the same outcome. I've use a 2012 no problems like Harley or mine do happen. With 2013, I get the

 

This has been frustrating for Harley

 

On the Loft ProblemX.ics file, Part51 was from Harley and Part56 is what I did. The only way the I was able to unfold it was using the Solid/Surface Flat Pattern from Faces tool the created Part7

 

 

 

 

Joseph

Loft_problemX.ics

[HDEAR]

I have to file this to bug reports and hopefully a resolution can be made. I am experiencing what Harley has been doing and I am coming up with same results also with Dariusz video. I have tried it with my other notebook running 2014 also with the same outcome. I've use a 2012 no problems like Harley or mine do happen. With 2013, I get the

 

This has been frustrating for Harley   

 

On the Loft ProblemX.ics file, Part51 was from Harley and Part56 is what I did. The only way the I was able to unfold it was using the Solid/Surface Flat Pattern from Faces tool the created Part7

 

 

Joseph

38376[/snapback]

 

Thanks Joseph. Appreciate the promptness and honesty.

[dleczynski]

Thank you.  I followed your instruction exactly.

 

Unfortunately, when it came to the unfold, all I got was the line as shown below.

 

So something's happening when I hit the unfold button.  It maybe a setting I have wrong or one simple step during the loft build process, however I have now followed several sets of instructions and got the same 1 line result when pressing unfold.

38375[/snapback]

 

all is well, but IronCAD depending on the version has different tastes. The 2014 version of the sheet develops modeling kernel ACIS.

 

Select the part, make a shortcut CTRL + K. Sheet changes color and unfold.

[jolizon590016]

Hi Dariusz,

 

That work and I hope it works for Harley too

 

 

Should we set something for Default Kernel or run Ctrl+K on sheet metal projects?

 

Likewise I can't generate the bend lines

 

Again Thank you

 

Joseph

LoftSheetMetalck.ics

Edited August 4, 2014 by jolizon590016

[dleczynski]

Hi Dariusz,

 

That work and I hope it works for Harley too 

 

 

Should we set something for Default Kernel or run Ctrl+K on sheet metal projects? 

 

Likewise I can't generate the bend lines

 

Again Thank you

 

Joseph

38379[/snapback]

 

the show was made ​​a rectangle with rounded corners (geometry similar to the circle). If you perform the transition from the upper circle (circle) it will not be bending line.

 

IronCAD 2013 version to work correctly on Parasolid. Therefore, you can specify an where well where wrong. The same spring running slow on ACIS 2014. Parasolid very quickly.

LoftSheetMetalck.icd

LoftSheetMetalck.ics

Edited August 4, 2014 by dleczynski

[jolizon590016]

Was able to finally display the Bend line display at ICD

 

 

LOFTSHEETMETALCK.PDF

Edited August 4, 2014 by jolizon590016

[HDEAR]

the show was made ​​a rectangle with rounded corners (geometry similar to the circle). If you perform the transition from the upper circle (circle) it will not be bending line.

 

IronCAD 2013 version to work correctly on Parasolid. Therefore, you can specify an where well where wrong. The same spring running slow on ACIS 2014. Parasolid very quickly.

38380[/snapback]

 

Just so I am understanding you correctly;

 

When performing the loft, you must choose the rectangle first, then the circle - correct? That will ensure you end up with bend lines - correct?

 

When performing the unfold, you must click on the part ( Cyan outline ), press CTRL-K and then perform the unfold - correct?

[jolizon590016]

Hi,

 

I am getting this:

 

 

From the attached ics file. It does preview and create the bend lines but doesn't produce the manufacturing data on the icd sheet.

 

Also attached is draft pdf

 

Loft_to_sheetmetal_quick_guider1.pdf

 

I also generated a side by side file comparison on icd between the 2 files

 

 

I also tried to edit the cross section 2 of sheet metal loft1 from LoftSheetMetalck.ics file just to see if the over lapped message has to something to do with it. But why does Cross-Section number: Bad Cell instead of the Profile#

 

 

Is this an indicator of a bad geometry creation or something that requires a mid section to loft with.

 

Thanks, Joseph

Rect2Circ.ics

Edited August 4, 2014 by jolizon590016

[mwalls558626]

Just a note to all using Sheet Metal Loft. What I have found is that if you are doing the Loft function in sheet metal, you need to make sure your flat pattern is true, to the normal x,y,z coordinate system, in order to get the bend line information to come out correctly. If there is any "angle" to the flat pattern, looking at the thickness of the sheet metal, away from a normal xyz coordinate system, you will not get the bend line information to come out correctly.

 

If you take the flat pattern and make a quick drawing with the 3 normal views, then if you look at the view that looks normal to what would be the thickness of the material, and it is not straight along the axis, you will more than likely not get the bend info on the sheet.

 

Mike

[jolizon590016]

Hi Mike,

 

Tried to do as told. I got the position By Angle 80.532 so I subtracted it to 90 and got a difference of 9.462. What I was accustomed to doing is on the brep created by the unfolded part on the IntelliShape level, I rotate associated anchor point use the Triball, switch off the TriBall. And next what I do is select the brep again and tick of the anchor till it turns yellow and activate the TriBall to rotate if counter clockwise rotation of 9.462 so the anchor indicator will point at the right angle. So now it really face flat from the front view.

 

I do it the other way if I want to maintain it original position when it was created and do the same on the part level so when I create a catalog part of an assembly I don't have to deal with the angle to reposition when it was drop back to the scene.

 

As for this files it still shows the bend lines only even when it is really flat now at the front view. What I did found out is if the transition has 2 parallel adjacent sides, works perfectly. As you said it is flat when it unfolds from the adjacent face.

 

Just a side note I really like using IC than anything else. In the past I have to work with SolidEdge which had a steep learning curve, but found IC .x_t neutral parasolid file exchange working perfectly with it with out reorienting position and missing data that needs to generated unlike with SWX http://www.ironcad.com/support/community/s...icons/icon8.gif sorry about that.

 

I use the SE drafting component as required by the office for part of its documentation standard an found it can generate easily the files from IC and easily pick up data from it to use with the 2D annotation than ICD which I wish it could do. I was doing playground equipment that time and have to use a lot pipes for hand rails and creating centerline was easier.

 

Still searching for the right process.

 

Regards - joseph

Sq2Circ_8462.ics

Sq2Circ_8462.icd

[jolizon590016]

Mike,

 

My apologies that I placed my thoughts right away. The process that I did is good for the scene and for catalog content items.

 

I sensed there is more too it on what you have written. Instead of struggling to use Look At (F7) or as the process I am accustomed to, logic escapes me that using the Auxiliary View will solve this and it did. I just have to make sure that cursor highlights a green short parallel indicator rather than a point so it will be line on rather say spot on.

 

 

 

Thanks for your assistance this an to the rest of the community. The only thing left I can not figure out will be the bad cell thing.

 

Regards - joseph

 

SQ2CIRC_8462.PDF

Sq2Circ_8462.ics

Edited August 6, 2014 by jolizon590016

[jolizon590016]

I will post the finished guide to Tips and Tricks section and at GrabCad. Thank to all who helped with this thread.

Edited August 6, 2014 by jolizon590016

[Jonas@Solidmakarna]

You mentioned "struggling with F7", but I think the easiest thing to do is to use the "Look at" tool (F7) in the Scene, then use the option "From Scene" when you create the view. That has been working very well in cases like this for years.

[Robert Andersson]

Also in similar cases when you need to adjust the view, select the part, Triball on, RMB and select "Orient Triball to Global". This will orient the part to the scene XYZ.

 

You mentioned "struggling with F7", but I think the easiest thing to do is to use the "Look at" tool (F7) in the Scene, then use the option "From Scene" when you create the view. That has been working very well in cases like this for years.

38404[/snapback]

 

[Jonas@Solidmakarna]

Re-orienting unfolded sheet metal doesn't work, since it has a set orientation in space. It will move back to where it was. That's why F7 and From scene is so fast and easy to use.

[jolizon590016]

Thanks guys. That is why I am quite struggling is I can't to get it to work as in previous versions as I want to since I am so used to earlier versions that changes orientation on the scene from the camera setting when it had no camera picker options(Trispectives to ICv1.4). I must really getting rusty on this. I remember when I edit scene from the drawing I think Esc switches or x out you back to the drawing.

 

Do you have any ideas about the bad cell instead of profile on edit. Thanks for your feed back

Edited August 9, 2014 by jolizon590016