Round Holes in Curved Sheet Metal, Unfold or not?

[Brian Hiebert]

We design and build large conical hoppers. My current models use an SSP and equations to drive most of the variables. It's created in sections and patterned around. The panels overlap on each side and then bolt to another piece so my hole patterns must fit through at least two different parts. I've been creating the holes in the parts while unfolded. However, when flattening the part there is no longer any point of reference to the SSP such as center axis. So then the center for the circular or curved patterns is based only on the individual parts. Is there a better way? My concern with creating the holes in the folded or bent state would be a hole that wasn't actually round when export dxf to cnc. Maybe it would be fine....
I'll try to include a couple screenshots.

[berg_lauritz]

Do you use the hole wizard for the pattern?
It should work on a 3D surface:
https://www.javelin-tech.com/blog/2020/ ... 3d-sketch/

[Frederick_Law]

Could SW do "Cut normal to"?
That will cut hole on bend which stay round when flatten.

https://www.goengineer.com/blog/solidwo ... heet-metal

[Brian Hiebert]

Do you use the hole wizard for the pattern?
It should work on a 3D surface:
https://www.javelin-tech.com/blog/2020/ ... 3d-sketch/

I have never used hole wizard.

Could SW do "Cut normal to"?
That will cut hole on bend which stay round when flatten.

https://www.goengineer.com/blog/solidwo ... heet-metal

I usually select "normal to" when working with sheet metal. I know it is supposed to make the cut perpendicular to the piece but not sure if it also would keep the hole round. I'll have to experiment with that one.
How would you project a hole pattern onto a curved surface like that? Would you do an assembly cut?

[HerrTick]

I assume you know where the holes need to be in the formed state. For such cases I do something like this:

•In formed state, make tiny triangular holes with point at hole center.
•Capture hole centers and surface normals with 3D sketch
•Unfold
•Make holes
•Fold

[Frederick_Law]

How would you project a hole pattern onto a curved surface like that? Would you do an assembly cut?

I don't use "assembly cut" unless it's part of production process.
I use Master Sketch, so I'll have holes center locations already in Master Sketch.
A pattern with equation to drive number of holes is probably what I'll use.
Cut one hole and pattern along.

Normal cut supposed to retain the cut profile to flat.
Worse case, cut smaller holes. Use them to get center in flat and recut with correct size.

[berg_lauritz]

I made this gif to illustrate the difference between the normal cut from one plane to using a 3D sketch for the hole wizard:

It depends on what your goal is. If you put fasteners through those holes it's probably a good idea to use the hole wizard for the holes where your fasteners are normal to. You can easily pattern the fasteners afterwards & it does not brake any mates when using it - plus with the 3D sketch possibility you don't have to align the fasteners anymore.
Always use the hole wizard for the holes where your fasteners are normal to!

[Brian Hiebert]

I assume you know where the holes need to be in the formed state. For such cases I do something like this:

•In formed state, make tiny triangular holes with point at hole center.
•Capture hole centers and surface normals with 3D sketch
•Unfold
•Make holes
•Fold

I wondered if this would be an option and hoped there was a better way...

I made this gif to illustrate the difference between the normal cut from one plane to using a 3D sketch for the hole wizard:

hole wiz and normal cut.gif

It depends on what your goal is. If you put fasteners through those holes it's probably a good idea to use the hole wizard for the holes where your fasteners are normal to. You can easily pattern the fasteners afterwards & it does not brake any mates when using it - plus with the 3D sketch possibility you don't have to align the fasteners anymore.
Always use the hole wizard for the holes where your fasteners are normal to!

Thanks! I'll have to experiment with the hole wizard. And see how it works on a curved surface!

[Brian Hiebert]

I don't use "assembly cut" unless it's part of production process.
I use Master Sketch, so I'll have holes center locations already in Master Sketch.
A pattern with equation to drive number of holes is probably what I'll use.
Cut one hole and pattern along.

Normal cut supposed to retain the cut profile to flat.
Worse case, cut smaller holes. Use them to get center in flat and recut with correct size.

I'm wondering if you could elaborate how you would do a master sketch of hole pattern in a conical shape?
Still a bit stumped on how to go about this.
Was on the phone with GoEngineer this morning and really didn't come up with anything better than what's been mentioned here. Goal is for all holes in multiple layers to stay aligned as model changes (I do a pack and go and change overall dimensions and angles for every customer)
Currently I unfold the pie shaped sheet, make an intersecting line colinear with edges and dimension holes from there and try to pull all angles and dimensions into the other parts. What I'm wondering if I still do the same with sheet but instead of sketches in flat patterns for the other parts, try to project holes from one sheet through the other parts in the assembly. How could I do this? Then I would still have to recreate the holes in flat pattern for the true diameter.......

[AlexLachance]

Hey Brian, do you have a sample file you could share? I do a lot of sheet metal and we've had occurences like this.

Depends on what are your needs also. In our case, we needed to have round holes with a constant spacing between them.

[Frederick_Law]

A few questions:
Are holes cut on the flat? So they're not "true round" after forming?
Are the plate thick enough that after forming/rolling the bolt won't go through? If so, need to cut oblong instead of round hole.

SSP use planes, Master Sketch use sketches.
You can add sketch to SSP and share them to all the parts.
Share center points so you can add hole feature on sheetmetal part.
Center points should be on mating plane.

[Brian Hiebert]

A few questions:
Are holes cut on the flat? So they're not "true round" after forming?
Are the plate thick enough that after forming/rolling the bolt won't go through? If so, need to cut oblong instead of round hole.

Holes are cut with CNC plasma. Sheet is not that thick that forming makes a measurable difference. It's only that if my software sees the the hole as line segments instead of arcs it does not make a smooth cut.

[Krzysztof Szpakowski]

A few questions:
Are holes cut on the flat? So they're not "true round" after forming?
Are the plate thick enough that after forming/rolling the bolt won't go through? If so, need to cut oblong instead of round hole.

Bravo, Frederick, I wanted to write that myself.

Holes are cut with CNC plasma. Sheet is not that thick that forming makes a measurable difference. It's only that if my software sees the the hole as line segments instead of arcs it does not make a smooth cut.

Not only the thickness is a problem here, but also the bending radius! If you cut a hole on a flat sheet as a circle and then bend/roll it, its diameter in the axis transverse to the bending axis will change. It's normal. Just like the fact that the hole is made in a 3D model and developed as an oval.

[TTevolve]

If you want actual holes in your flat pattern you will probably need to make them on the flat pattern you are cutting out.

On tis part the holes are partially in the bend

Here is what our laser software produced for the flat

You can see because the holes is partially on the band it flattens the one end because when it's bent it would stretch that end of the hole. IN pratice it doesn't come out perfectly round. In this case it's fine for what I needed on this part, but in other cases I would remove the ob-round holes and put an actual circle and then burn that if it had to be round. But when you form it the hole will no longer be true circle.

Ultimately, you need to figure out if the form, fit, and function require the perfectly round hole, since that would take some kind of secondary operation to achieve.

[Krzysztof Szpakowski]

because when it's bent it would stretch that end of the hole.

Not completely. It is stretched and compressed at the same time. Depending on whether it is the outside or inside of the bend.

[Brian Hiebert]

l really don't care what shape the holes are. But my plasma does. If in flat pattern export it's not round, my Plasma software sees it as a bunch of little lines and treats it differently. Had an issue just now with exporting 3 of my parts. Some were perfect and some exported the holes as not round. After spending some time with SW support he determined the error was with the Sketch used to create the lofted bend. Somehow in the folding and unfolding of the part, even though everything worked and displayed correctly, SW would change the hole to a spline! And of course to recreate the initial sketch would basically mean starting over with the part. Holes were fine until the Fold command so I just suppressed everything below that, created a couple of my "etching" sketches again on this face and exported it that way.

[Brian Hiebert]

Now for the future, I did a little experimenting.... If I created the 3 or 4 sheet metal parts that have to have aligned hole patterns as ONE multibody part I can use ONE sketch to cut holes through them all. It appears like it is possible, however each body has to unfolded and folded separately. As long as they stay aligned when unfolded I should be good. And in the drawing it appears I can only pick one body at a time it I want the flat pattern view. Any Advice for me on this?

Another frustration, My plasma is capable of etching lines, so I just sketch the lines I want etched and export as a different layer. I have been creating them in the flat pattern config so they show in the flat pattern drawing. However, anytime I edit the part and create any editing between the unfold/fold feature it breaks all relations in the sketches made in flat pattern......Is there a better way to do this? For some reason I thot a sketch made in the normal config didn't show properly in the flat pattern but a little experiment I did here looks hopeful...

[TTevolve]

Now for the future, I did a little experimenting.... If I created the 3 or 4 sheet metal parts that have to have aligned hole patterns as ONE multibody part I can use ONE sketch to cut holes through them all. It appears like it is possible, however each body has to unfolded and folded separately. As long as they stay aligned when unfolded I should be good. And in the drawing it appears I can only pick one body at a time it I want the flat pattern view. Any Advice for me on this?

Another frustration, My plasma is capable of etching lines, so I just sketch the lines I want etched and export as a different layer. I have been creating them in the flat pattern config so they show in the flat pattern drawing. However, anytime I edit the part and create any editing between the unfold/fold feature it breaks all relations in the sketches made in flat pattern......Is there a better way to do this? For some reason I thot a sketch made in the normal config didn't show properly in the flat pattern but a little experiment I did here looks hopeful...

Not sure if you can do it this way, but the part I showed above is a multi body part because it is a weldment. You can keep it multi body and make configurations where you use body delete/keep to get only the part you want and then su8ppress the others.