Dimensioning to holes in flat pattern 2

[prooney]

I've created a cylinder that is going to be made from plate and rolled which has pipes running into it and I need to dimension to the holes in the flat pattern view but I can't dimension to the holes in the flat pattern. Any ideas??

 

[JMirisola]

How did you create the holes? Do they appear in the flat pattern? Can you provide the model or screen shots?

Jeff Mirisola, CSWP
Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[EEnd]

Check out:
thread559-192763

Eric

 

[prooney]

I created the holes in the formed state. The majority of them have their centerlines intersecting the cylinders centerline with one hole perpendicular to the cylinder centerline.
We make ASME code vessels here so I put the nozzles in the piece while it's formed. From reading the other thread it doesn't look as though there is really an easy solution to this. Am I correct in assuming this.

 

[SBaugh]

Did you unfold the SM part first, make the hole, then refold the file back? This is proper procedure.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[prooney]

No I put the holes in before it was rolled. I put the holes in after the unfolding the part but they never showed up in the flattened state. Should they have?

 

[SBaugh]

If you put it after the Flat Pattern feature then you won't see it. You must us the Unfold, Fold features

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[prooney]

If I unfold the part before i put my nozzles in and then put my nozzles in after unfolding position, to me that defeats the purpose of what I'm trying to accomplish.

I don't want to have to unfold the part and then add my nozzles in the flattened state. Am I looking at this incorrectly?

 

[CorBlimeyLimey]

If you created the holes in the formed state, they will appear as mis-shaped ellipses in the flattened state. To be able to place dimensions to them in the flattened drawing view, you will have to place sketch-points around the hole outline.

To find the major and minor axis points of the 'ellipse', draw a horizontal and vertical line close to the outline and create a tangent constraint. Then place sketch-points at the tangent intersection.

 

[JMirisola]

Bear in mind that there is a difference between 'Unfold' (fold and unfold can be found in the sheetmetal tools) and 'flatten'. Assuming that your nozzles need to go into actual round holes, you need to:
•create the cylinder
•unfold it.
•put in your holes.
•fold it.

At no point should you 'Flatten' it.

Jeff Mirisola, CSWP
Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[CorBlimeyLimey]

But if he places round holes between the Unfold and Fold state, he will end up with non-round holes in the formed state.

 

[prooney]

I understand that the holes won't be round that's not the important part of what I need. Typically we burn out plates on our plasma table and roll them into cylinders from that point our fabricators locate where the nozzles are going to be and then cut out the holes with a hand plasma.

This step is very time consuming and I'm trying to take this step out of the fabricators hands and put the holes for the nozzles in the formed state. I need the dimensions for our QC department so they check the location of the holes.

Essentially what I'm trying to accomplish is to speed up our fabrication process. Any step that I eliminate in the office speeds up the fabricators job and makes it easier for them. I'm okay with the holes be ellipses I expect I just want to be able to put dimensions to the holes for our QC department.

I hope this makes sense of what I'm trying to do. Is this the correct way?

 

[JMirisola]

If the holes don't need to be round after rolling, then unfold/fold is the way to go. This will give your QC department what they need to be able to measure the holes, prior to rolling the plate.


Jeff Mirisola, CSWP
Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[CorBlimeyLimey]

Agreed. Then the only 'problem' would be placing the holes in the correct positions while in the Unfold state.

 

[prooney]

So what your telling me is that I need to put the holes in the unfolded state? If so that seems like a lot of extra work and defeats the purpose.

 

[CorBlimeyLimey]

No, that is just one simple method of creating a circular hole which can be dimensioned to.

If you really want to place the hole in the formed state, then see my first post.

 

[Theophilus]

CorBlimeyLimey is right on this (so is Jeff, but you need to add the holes in the formed state). Follow his first post. If you like, make the holes added in the formed state a tad small--then make them perfect in the flattened state, using the formed holes as locators for the "perfect" holes. More time in the office, less time in production, right?



Jeff Mowry

http://www.industrialdesignhaus.com

What did you dream? It's all right--we told you what to dream.
--Pink Floyd, Welcome to the Machine

 

[prooney]

CBL, Do I place the points in the sketch after it's unfolded? I'm very new to using SolidWorks so forgive me for my ignorance to some of this stuff. I'm trying to learn trial by fire. Thanks for all the info it's greatly appreciated.

 

[Theophilus]

You may want to read up on the sheetmetal stuff in the Help files--good stuff to aid in learning (although you've probably done this a bit already).

The way I'd do it is add the sheetmetal feature after my holes are already formed. Roll back to a flattened state and create a sketch on the flat metal. You can create construction lines that are tangent to the edges of each holes--like a box around each hole--four construction lines. Create a vertical and horizontal construction line set to the midpoints of a vertical and horizontal box line. Where they intersect is your hole center. Create your circle/ellipse from that center point. Make sure your new holes actually cut some material, so that they're a bit larger than the original holes made during forming.

Later (I think) you should be able to dimension to your new holes in the flat pattern (in a drawing view).



Jeff Mowry

http://www.industrialdesignhaus.com

What did you dream? It's all right--we told you what to dream.
--Pink Floyd, Welcome to the Machine

 

[CorBlimeyLimey]

You could place the sketch-points in the model as Theo' suggests, and then Show the sketch (when in the drawing) for dimensioning to.

Or you could place them in the actual 2D drawing view of the Flattened part.