Tool ID selection

[Dave_Walker]

Quick question for NX Sheet Metal users...

Does anyone use the Tool ID Selection option in Sheet Metal Preferences-->Part Properties-->Parameter Entry? As part of our upcoming projects I would like to know if it is functionality that is actually used.

If you do, how do you factor for using the same tool with different material grades/types/thicknesses?

Thanks.

[Thomas_K]

Hi Dave,

nope, but I teach it in the trainings. Sometimes there are also Tooling guys, but I've never heard they use it in daily work...

Best Regards,

Thomas

[MMNH]

Hi Dave,

Nope, we do not use it. Reason is that we do not have in house manufacturing and therefore we need to stay as general as possible as tooling is concerned.

[RGudorf]

Dave,

We looked at it but for the reasons you are stating, it doesn't do enough for us. Over the last few BETA programs with Tony Salerno and his team, we discussed the need for a much more flexible (complex) system to deal with these issues. Anyone that actually designs and fabricates their own sheet metal deals with this on a daily basis. We are in the early process of developing our own system much along the lines of Frank Huysmans external system.

That process involves a cascading menu process tied to an SQL database that starts at the parts inception. 

1. Choose material from a list (we have over 200 types that we have fabricated)

2. Choose material thickness/gauge

3. Based on the above two choices the options for tooling combination can be significantly narrowed via the system. It won't let you pick a tooling combination that can't be used with the fist two choices.

4. We are looking at two methods here, pick tooling and an I.D. bend radius is fed into the Sheet Metal Preferences. Or we will be given a list of available bend radii to choose from that can be generated based on the tooling we own, and then the tooling combination will be populated.

5. All the above choices will then be pushed into the appropriate fields so that the part is automatically generated at the proper thickness, bend radius and appropriate attributes are populated to the titleblocks, notes, etc.

HTH,
Ryan

[Dave_Walker]

Ryan,

Thanks for the feedback here.  It does look like current projects may satisfy your requirements without the need for external databases.

[RGudorf]

Dave,

That sounds very promising to have something internal that would take care of our needs. Feel free to contact me with any questions you might have concerning this process.

Thanks,
Ryan

[Dave_Walker]

Sure, when we have something that the development team are happy with we may be able to share our intent - or at least hint at what is proposed.

[frank_nx]

Hi Dave,

Some years ago I looked at it.

To be very short about it;

The dialog is asking the questions that need to be the answered.

This is what the dialog looks like now:

Sheet Metal Tool ID Selection Dialog Boxd ID

I would rather see a dialog that asks me:

1. Material Type
2. Material Thickness (that is avalaible for the choosen Material Type)
3. Bend Tool Setup (that is physically available AND functionally possible for that given Material Type/Material Thickness combination)

The result in the 3D Sheet Metal design should be a specific Bend Radius and Specific Bend Neutral Factor according to the bend angles that are present in the design.

btw Bend Radii tend to get bigger with larger inside Bend Angles.

As the dialog is now it is as if we can oblige the material to be formed with a bend radius as we would like. In reality this is not possible with air bending = press brake bending.

The only way of forcing a specific Bend Radius would be by "bottoming" -meaning that the punch forces the sheet metal plate fully down in the die- like stamping.

Since the existing dialogue can't do this I stopped investigating this any further and decided to do it our own way. (BTW it's the same method that e.g. Trumpf and LVD use. I bet there will be other press brake manufacturers that use the same method)

In general the design and the tools being used dictate what the resulting bend radii will be.

NOT the other way round. This is where almost any CAD system fails. In fact I don't think that there is a CAD system at this moment that does this correctly OOTB.

Maybe SWX in combination with an add on called TopsWorks.

And also TruTops Boost in combination with SpaceClaim.

[RGudorf]

Frank,

Did you mean the dialog is NOT asking the questions that need to be answered? Or it does and it should be another way? I think we are both on the same page although we may get to our flat patterns differently. And we also refer to "bottoming" as "coining" at least in the States as far as I know.

Best Regards,

Ryan

[frank_nx]

Hi Ryan,

Correct; the dialog is asking for imput that I'm actually looking for.

Since a Bend Radius is the RESULT of a chosen Material Type - Material Thickness - Bend Tooling - designed Bend Angle, it seems rather strange to me that you need to provide a bend radius yourself.

Also given the fact that a bend radius tends to get bigger when the inside bend angle gets bigger.

Here are some random values that I've taken from our database (for a given material and tool setup):

Inside bend angle	Material Thickness	Bend Allowance	Back Gauge Correction	Inside Bend Radius
90	2	3.75	-1.875	2.15
105	2	2.59	-1.295	2.38
120	2	1.77	-0.885	2.72
135	2	1.15	-0.575	3.38
150	2	0.67	-0.335	4.91
165	2	0.28	-0.14	9.67

Our database now contains almost 50000 lines and it will grow everytime we bend something new.

You might also notice the mentioning of "Bend Allowance " instead of a

"Neutral Factor"

I would also like to see the possibility to use a Bend Allowance for making bend corrections.

A Bend Allowance is a correction DISTANCE that you need to deduct from the sum of the desired outside flange dimensions. This means that this is a value that can be measured directly from a bend test. It is very direct and straightforward.

Working with a Neutral Factor always means that you need to calculate.

I hope this helps

[Dave_Walker]

Quick question for NX Sheet Metal users...

Does anyone use the Tool ID Selection option in Sheet Metal Preferences-->Part Properties-->Parameter Entry? As part of our upcoming projects I would like to know if it is functionality that is actually used.

If you do, how do you factor for using the same tool with different material grades/types/thicknesses?

Thanks.