Rolled Sheetmetal Part w/Holes 9

[Stugots]

I am helping a coworker and have a rolled sheetmetal part with cut holes in it. I can not dimension them in the flat pattern in a drawing. I can't select the holes in the flat view..."The selected entities could not be converted into a line or arc." is what I get. I've tried holding the "SHIFT" key down and no luck.

I understand that it is not making the hole axis perpendicular to the flat pattern plane so it is making the circle into segments. Is there a way around this?

On a side note: Solid Edge doesn't have a problem with this sort of thing because you are able to flatten sheetmetal by selecting either a face or "PLANE" for your flat and then blow holes in it and it forms the holes onto your bend when you suppress the flat. Am I missing something here? Please view the part model path below.

http://www.mooload.com/new/file.php?file=file01/190707/1184875991/441-53-9-13.SLDPRT&s=t

Stugots
Mechanical Designer
SW '06 SP5.1

 

[robnov77]

If you put in a round hole when the sheet is rolled it will not be round when it is un rolled and vice verca.

 

[CorBlimeyLimey]

Unfold
Insert holes
Fold

 

[Stugots]

Yes, I understand the premise of a round hole in a formed sheet to a flat distortion factor. What I am really asking is why does SW have such a problem recognizing the hole in a flat pattern when you try to dimension it.

My only solution so far is to actually have to sketch a circle on top of the hole in the drawing and dimension to that. Kinda defeats the parametric advantage of this software because the sketches don't move with the holes when updating.

Stugots
Mechanical Designer
SW '06 SP5.1

 

[CorBlimeyLimey]

How is the part actually being made? Are you machining the holes in the rolled part or the flat part? If in the flat, then create and dimension them in the flat.

Try selecting View > Temporary Axes and dimensioning to them.

 

[engAlright]

In the part model posted, the hole features have been added as round in the "formed" config, so they will not appear as round holes in the flat pattern - this is why you can't dimension them...because they are splines in the flat pattern, and you can't really dimension splines in the normal fashion.

If you want them to be round holes in the flat pattern, you have to follow CBL's suggestion and add an unfold feature, then add the the holes, then add a fold feature. Or...you can add the holes in between the flatten bends and process bends features.

 

[Stugots]

CBL: They want to laser cut the holes in the flat. The holes were created in the formed state "part in place" in the assembly because of it's relations to mating parts. I would have thought you could place 3D points on the part in the assembly then flatten and place the holes in the flat, but because of SW flat orientation "lack of being able to flatten to a plane" the 3D points would be out in space and useless because they loose their orientation to the "surface" they were sketched on.


Unfortunately Temporary axis shows nothing in the flat view in the drawing.

Stugots
Mechanical Designer
SW '06 SP5.1

 

[engAlright]

If they are laser-cutting the holes can they just nest directly from the drawing or a converted dwg? We no longer include dimensions such as this in our drawings for laser-cut parts precisely for this reason - the requirement for including dimensions greatly limits what you can design, and we can nest directly from a converted DWG anyway.

If you absolutely need to have holes that look round in the formed and flat configs, you will have to add additional "round" hole features to the flat pattern based off of the locations of the features in the formed config.

 

[ShaggyPE]

I am in agreement with engAlright. Do you desire round holes when the part is rolled, or round holes when the part is flat. It seems to me from your description of the assembly that you want round holes when it is formed. Then dimensioning the holes as a spline in the flat seems acceptable.

-Shaggy

 

[Stugots]

engAlright: The idea of taking dimensions off the flat patterns has been proposed here. My counter point would be, how would quality check the part before they possibly waste the man hours in forming if the part is wrong unless the dwg is then dimensioned? Is this as issue there?

Stugots
Mechanical Designer
SW '06 SP5.1

 

[Stugots]

Shaggy: SW won't let you dimension the holes as a spline in a flat. When you pick it you get: "The selected entities could not be converted into a line or arc."

Is there a special way to dimesion a spline?

Stugots
Mechanical Designer
SW '06 SP5.1

 

[dgowans]

Stugots,

It sounds to me that you need circular holes in the flat but want circular holes in the formed. Is that the case?

If so, you will have to do one of 2 things:

1) As previously stated, create 2 configs of the part - one for detailing and one to use in your assembly.

2) Create the part with the circular holes in the flat, allow them to deform when the part is rolled, and add reference geometry to the formed part to facilitate mating in your assembly. Creating the reference geometry might be a real PITA, but this method will be more reflective of the physical world.

 

[engAlright]

When there are no dimensions on the flat your only realistic option for checking quality is using part templates. However because the laser cutting process is entirely automated there is little that goes wrong if the nesting is done correctly...

We do large weldments with fairly broad tolerances (+/- 16th) so at the end of the day as long as the part fits in the weldment it works.

 

[Stugots]

Thank you one and all for all your time.

Stugots
Mechanical Designer
SW '06 SP5.1

 

[Updraft]

We do as engAlright - we do not dimension the flat. Our justification is this: What we want is the final shape as defined in the formed part and by its dimensions. We don't "really care" about the flat so long as we get the final formed part. The flat pattern is merely something along the way you have to do to get to the final product.

For this reason we also have established as our standard operating procedure that we design the formed part then convert it to sheet metal, rather than start with a sheet metal feature and add bends or flanges. By starting with the formed part if we decide to change the gage or bend radius, but we have defined the formed part according to our design intent (such as controlling the outside width of opposing flanges that go inside another part where we are controlling the inside width of its flanges) then our flat pattern is automatically and appropriately updated. If we had started it as a sheet metal part it would be like redesigning the part to get everything to line up again. Design intent, baby!!

And since, like engAlright, we feed the flat pattern directly to our auto nesting software from SWX (no making of an intermediate DXF, thank you) we do not need to dimension the flat at all on the drawing. All we do with the flat on our drawings is show bending information. On occassion we will supply a few reference dimensions, but this is mostly to help distinguish between two parts that are similar.

- - -Updraft

 

[Stugots]

Updraft: Can you explain how to convert from a solid extrusion to a sheetmetal part? I've been spoiled by Solid Edge and it was a simple button click, but I haven't been able to find anything in the help files on this topic.

Stugots
Mechanical Designer
SW '06 SP5.1

 

[JMirisola]

Create the extrusion, leaving a gap. On the sheetmetal toolbar is the button you're looking for...'rip'.

Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP2.0, Dell M90, Intel 2 Duo Core, 2GB RAM, nVidia 2500M

http://designsmarter.typepad.com/jeffs_blog

 

[Updraft]

Stugots,

SWX has the absolute best help file / tutorial of any software I have seen. Go to SWX Help, Index, and look for Sheet Metal Design Methods. It discusses designing a part starting from sheet metal as well as designing it then converting it to sheet metal.

The only real "trick" to designing it then converting it is keeping the material thickness the same from feature to feature and then making sure that thickness matches your standard for the particular gage of metal. We design using a lot of open sketches (thin feature) and thicken them upon making the feature (much faster than drawing every little edge!). Leave sharp corners where the part will be bent; the software adds the proper radius features and bend relief when you convert it to sheet metal.

Try it, you'll like it.

- - -Updraft

 

[Stugots]

Updraft: I have a bad habit of trying to use the search in the SWX help and it greatly limits the findings. I'll use the index from now on. Thx

Stugots
Mechanical Designer
SW '06 SP5.1

 

[Stugots]

Updraft: I am trying to follow the Sheetmetal/Design methods/design a part from the flattened state, then convert it to sheet metal.

Doesn't work how they have it written. I think there is something missing between steps 4 & 5. Any ideas?



Stugots
Mechanical Designer
SW '06 SP5.1