I'm looking at an opportunity to save time on drafting parts for my company. Currently we dimension all features in the flat as well as the formed part. To me this can be excruciating when trying to layout a part that has a lot of features in it. I just want thoughts on why dimensioning for flat pattern parts is not necessary maybe other than for secondary operations like tapping, c'sinks, etc. We make all of our own parts and are in charge of the software and laser. To me, we are wasting too much time on something that can be validated in a few simple steps.
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Why dimension sheet metal in the flat
- Thread starter STeliczan
- Start date
We quit dimensioning flat parts years ago. This is what is referred to as minimum content drawings, reduced dimension drawings or model based definition. The math data controls the geometry.
All I show is basic overall size so the operators know how big a sheet of material to throw up on the laser table. I will dimension any critical features that I would like to have inspected on the flat if it is important to form, fit or function. Otherwise, I know our laser is more than capable of producing the geometry within the general tolerances the part needs for function.
Cheers,
Anna Wood
SW2014 SP2, Windows 7 x64
All I show is basic overall size so the operators know how big a sheet of material to throw up on the laser table. I will dimension any critical features that I would like to have inspected on the flat if it is important to form, fit or function. Otherwise, I know our laser is more than capable of producing the geometry within the general tolerances the part needs for function.
Cheers,
Anna Wood
SW2014 SP2, Windows 7 x64
MikeHalloran
Mechanical
Another reason for not dimensioning flats is that the dimensions you or your computer compute for the flat may not be capable of producing the part you want, depending on the actual material thickness and temper, the tooling available for the forming operations, and the skill level of the entire crew.
You have control over precisely none of that, so developing flats for other than illustrative purposes is a huge waste of your time, and dimensioning them more so.
Mike Halloran
Pembroke Pines, FL, USA
You have control over precisely none of that, so developing flats for other than illustrative purposes is a huge waste of your time, and dimensioning them more so.
Mike Halloran
Pembroke Pines, FL, USA
STeliczan,
In general, you should dimension only the folded/finished part since that is what you ultimately want. It is up to the fabricator to deliver the finished part. The flat patterns required to deliver that will differ from shop to shop simply due to differences in equipment alone, not to mention material variations.
That being said, you apparently also have responsibility for the fabrication and the flat pattern is therefore your important starting point. But this raises a couple of questions:
1. Have you done a study to determine your bend calculations, i.e., have you determined k-factors or bend deduction tables for the various combinations of material, temper, thickness, bend radius? If you have not then you must basically stop what you are doing in the shop and get that information. With it SWX will generate an accurate flat pattern. Without it SWX will generate a close flat pattern that can frustrate the bending operations.
2. What are you using to program your punching and bending operations? Are you using something that will take a 1:1 DXF of the flat pattern and program the punch press or are you manually programming the press from a detailed drawing of the flat. If the latter then you are stuck with having to generate detailed dimensioned drawings of the flat pattern. If you are using the former then about the only dimensions needed on the flat pattern are the tapping notes (thread callouts, but not locating dimensions) or any other instructions on things that must be performed after punching but prior to bending such as Pemserts. You might also show overall size, but that is merely for reference. Other than that the only other dimensions that might be needed on the flat pattern are the bend lines.
In general, less is better so long as it is clear and adequate. Do not add any more dimensions than necessary. As I re-read your original post I would expect that you could eliminate a ton of unnecessary work by omitting dimensioning the flat pattern and just leaving the tapping and bending notes.
- - -Updraft
In general, you should dimension only the folded/finished part since that is what you ultimately want. It is up to the fabricator to deliver the finished part. The flat patterns required to deliver that will differ from shop to shop simply due to differences in equipment alone, not to mention material variations.
That being said, you apparently also have responsibility for the fabrication and the flat pattern is therefore your important starting point. But this raises a couple of questions:
1. Have you done a study to determine your bend calculations, i.e., have you determined k-factors or bend deduction tables for the various combinations of material, temper, thickness, bend radius? If you have not then you must basically stop what you are doing in the shop and get that information. With it SWX will generate an accurate flat pattern. Without it SWX will generate a close flat pattern that can frustrate the bending operations.
2. What are you using to program your punching and bending operations? Are you using something that will take a 1:1 DXF of the flat pattern and program the punch press or are you manually programming the press from a detailed drawing of the flat. If the latter then you are stuck with having to generate detailed dimensioned drawings of the flat pattern. If you are using the former then about the only dimensions needed on the flat pattern are the tapping notes (thread callouts, but not locating dimensions) or any other instructions on things that must be performed after punching but prior to bending such as Pemserts. You might also show overall size, but that is merely for reference. Other than that the only other dimensions that might be needed on the flat pattern are the bend lines.
In general, less is better so long as it is clear and adequate. Do not add any more dimensions than necessary. As I re-read your original post I would expect that you could eliminate a ton of unnecessary work by omitting dimensioning the flat pattern and just leaving the tapping and bending notes.
- - -Updraft
This is something I have found difficult to adapt to. Time has changed the technology available, and the workflow that designers should use is different now. The sooner I adapt, the better my work will be.
Early on in my career, I was building parts to fully dimensioned flat patterns. Many were hand-drawn. I could use AutoCAD but I was encouraged to make carefully scaled flat patterns. I used a manual shear and brake so the 1:1 flat pattern made the job easy. Nobody had parametric CAD but AutoCAD the flat 2D patterns were very accurate. I didn't realize at the time that the kinds of parts I made were being designed with relatively few critical interfaces that had to line up, and in a lot of cases parts with virtually no holes at all were just drilled upon assembly by matching holes in the mating parts. Today, much more is expected of our sheet metal parts. The "old way" is still adequate when doing repairs, for instance, but the "new way" can do that better, too.
As I became the parts designer, and later still when I started using 3D paramatric CAD (Inventor) the workflow changed. A properly dimensioned 3D sheet-metal finished part is sufficient to completely define both the end product that was needed, and the layout of the flat pattern. But old habits die hard. I would be caught many times dimensioning the flat patterns in great detail, but sending off the flat-pattern in a DXF anyway. The operator of the router table wouldn't look at my dimensioned drawing because he had all the numbers in the DXF, so those dimensions were moot. Then the part would be bent according to the scant dimensions on my 3D finished part drawing views, and come out wrong in the end inspection. Often on things like corner relief that Inventor doesn't model very cleanly.
So it's a shift in the frame of mind, and people insisting on the flat pattern dimensions are relying upon a way of designing parts that just isn't appropriate to the current world of router tables and NC brakes.
STF
Early on in my career, I was building parts to fully dimensioned flat patterns. Many were hand-drawn. I could use AutoCAD but I was encouraged to make carefully scaled flat patterns. I used a manual shear and brake so the 1:1 flat pattern made the job easy. Nobody had parametric CAD but AutoCAD the flat 2D patterns were very accurate. I didn't realize at the time that the kinds of parts I made were being designed with relatively few critical interfaces that had to line up, and in a lot of cases parts with virtually no holes at all were just drilled upon assembly by matching holes in the mating parts. Today, much more is expected of our sheet metal parts. The "old way" is still adequate when doing repairs, for instance, but the "new way" can do that better, too.
As I became the parts designer, and later still when I started using 3D paramatric CAD (Inventor) the workflow changed. A properly dimensioned 3D sheet-metal finished part is sufficient to completely define both the end product that was needed, and the layout of the flat pattern. But old habits die hard. I would be caught many times dimensioning the flat patterns in great detail, but sending off the flat-pattern in a DXF anyway. The operator of the router table wouldn't look at my dimensioned drawing because he had all the numbers in the DXF, so those dimensions were moot. Then the part would be bent according to the scant dimensions on my 3D finished part drawing views, and come out wrong in the end inspection. Often on things like corner relief that Inventor doesn't model very cleanly.
So it's a shift in the frame of mind, and people insisting on the flat pattern dimensions are relying upon a way of designing parts that just isn't appropriate to the current world of router tables and NC brakes.
STF
DiegoLGraves
Mechanical
It depends on the inspection requirements in your shop, for your vendors, and for your customers. If your shop fully inspects the part before it's formed they will need the dimensions and/or a reliable way to inspect the part, such as a Virtek laser scanner or CMM. Our engineering department provides laser scanner programs to check the flat parts before they move to forming. It's not unusually for a cutting machine to miss a hole or have a part or sheet shift while in process, so we try to stop the parts in production before more work is put in. Also a great many of our customers, from military products to point of purchase customers require inspection reports. The requirement for these types of reports has gone through the roof in the last 4 years. Some of the information for these reports can be gathered early in the process rather than at the end when the parts are ready to ship.
You need to support your existing processes along with developing newer processes for your current and future technology capabilities. If you need the info for checking the flat patterns it's better that the engineer/designer provides it than having the shop do their own calculations off of the folded views. The information the fabricator uses may be different - either better or worse - than what you are using to develop the flats.
But yes, it can be a pita, 2 cents worth, Diego
You need to support your existing processes along with developing newer processes for your current and future technology capabilities. If you need the info for checking the flat patterns it's better that the engineer/designer provides it than having the shop do their own calculations off of the folded views. The information the fabricator uses may be different - either better or worse - than what you are using to develop the flats.
But yes, it can be a pita, 2 cents worth, Diego
davidinindy
Industrial
We draw up the final result, that we want to receive, and leave it to our vendors to be the sheetmetal experts, and know what their machines and personnel are capable of.
Often, us designers don't know who will be making our parts, so we can't design to any particular shops equipment.
David
Check out my professional profile and connect with me on LinkedIn.
Often, us designers don't know who will be making our parts, so we can't design to any particular shops equipment.
David
Check out my professional profile and connect with me on LinkedIn.
STeliczan (Mechanical) (OP)
As Diego Graves said it depends on who your customer is. If you have a flat pattern going to a CNC punch, plasma torch, laser or water jet.
In order to get a tool path the operator very often has to remove dimensional data. On the other hand the press brake operator wants the dimension from the edge of the part to the centerline of the bend and how many degrees up or down the part is bent at what radius.
I end up doing a dimensioned drawing of the finished bent up part, and an un-dimensioned DXF file for the Water Jetter or other cutter out of the piece of metal. The flat pattern is generated as a courtesy to shops I know, and they use it at their own risk. If a dimensioned flat pattern with bending instructions is sent, it also goes with a warning that a flat pattern must be bent at the radius and angle specified or the dimensions will be in error. and that in all cases the dimensioned drawing of the bent up part rules.
I used SolidWorks for many years to do this, then later moved over to Geomagic Design which has the same K factor/ bend deduction capability as SW.
If the part is going to an unknown vendor , they just get the final assembled dimensioned view, until I have an idea of whether or not they even want the layout information.
B.E.
You are judged not by what you know, but by what you can do.
As Diego Graves said it depends on who your customer is. If you have a flat pattern going to a CNC punch, plasma torch, laser or water jet.
In order to get a tool path the operator very often has to remove dimensional data. On the other hand the press brake operator wants the dimension from the edge of the part to the centerline of the bend and how many degrees up or down the part is bent at what radius.
I end up doing a dimensioned drawing of the finished bent up part, and an un-dimensioned DXF file for the Water Jetter or other cutter out of the piece of metal. The flat pattern is generated as a courtesy to shops I know, and they use it at their own risk. If a dimensioned flat pattern with bending instructions is sent, it also goes with a warning that a flat pattern must be bent at the radius and angle specified or the dimensions will be in error. and that in all cases the dimensioned drawing of the bent up part rules.
I used SolidWorks for many years to do this, then later moved over to Geomagic Design which has the same K factor/ bend deduction capability as SW.
If the part is going to an unknown vendor , they just get the final assembled dimensioned view, until I have an idea of whether or not they even want the layout information.
B.E.
You are judged not by what you know, but by what you can do.
- Status
Similar threads
- victor andreevich
- DASSAULT: SOLIDWORKS 3D Design