How to make a jog where offset is less than material thickness?

[bnemec]

I cannot figure out how to make a jog where the offset is less than the thickness, nothing I have tried is working and I'm out of ideas. I even looked at the help page, it was most generic on the topic.

Thank you.

[mike miller]

Make sure your angle is shallow enough that the bend radii don't interfere. If that doesn't work, uncheck "Fix Projected Length". (Not sure why that last one makes a difference, but it does sometimes.... )

[bnemec]

Make sure your angle is shallow enough that the bend radii don't interfere. If that doesn't work, uncheck "Fix Projected Length". (Not sure why that last one makes a difference, but it does sometimes.... )

But I want the projected length to remain the same. Looks like toggling that off, then setting the angle then turning it back on works. seems really stable

It appears that SW "jog" fails if the bends touch, ie there must be some flat between them. Which tells me the "jog" feature is a glorified macro that combines two sketched bends?

[mike miller]

But I want the projected length to remain the same. Looks like toggling that off, then setting the angle then turning it back on works. seems really stable

It appears that SW "jog" fails if the bends touch, ie there must be some flat between them. Which tells me the "jog" feature is a glorified macro that combines two sketched bends?

The Jog feature isn't even 95% done, more like 75%. It likes to fail because it's derived from its cousin The Sketch Bend, which is the least stable sheet metal feature in SWX, at least IMO. Jog also tends to change face IDs at rebuild, even if nothing in it ever changed.

[mattpeneguy]

The Jog feature isn't even 95% done, more like 75%. It likes to fail because it's derived from its cousin The Sketch Bend, which is the least stable sheet metal feature in SWX, at least IMO. Jog also tends to change face IDs at rebuild, even if nothing in it ever changed.

If it worked correctly you'd get complacent...SW is just keeping you on your toes...

[HerrTick]

There's an persistent and pernicious dogma in CAD (not just SW) that sheet metal parts must consist of only sheet metal features from the sheet metal app. Utter tosh!

Z-bends (including jogs) are a great reason to ditch this dogma. In many cases, it is far simpler and better for the design (you know, the thing that matter most) to control a z-bend in a profile sketch and use conventional features. Double-true if mount/contact faces are on opposite faces.

Conversion to sheet metal can occur after key features are created. This feature is there in every CAD package. The only reason not to use it is one's own self-imposed limitations. We have enough limitations imposed upon us without creating our own.

[mike miller]

There's an persistent and pernicious dogma in CAD (not just SW) that sheet metal parts must consist of only sheet metal features from the sheet metal app. Utter tosh!

Z-bends (including jogs) are a great reason to ditch this dogma. In many cases, it is far simpler and better for the design (you know, the thing that matter most) to control a z-bend in a profile sketch and use conventional features. Double-true if mount/contact faces are on opposite faces.

Conversion to sheet metal can occur after key features are created. This feature is there in every CAD package. The only reason not to use it is one's own self-imposed limitations. We have enough limitations imposed upon us without creating our own.

That brings us to another thorny problem with SWX. Converting to sheet metal destroys the existing body and replaces it with a new one. ("Old things are passed away; behold, all things are become new." If only SWX didn't take the Bible so seriously.)

Anyhow, the implications for this are huge. If you have ANY references such as mates dependent on that part geometry before converting it to sheet metal, they will break. Even reversing a jog direction and rebuilding the Convert feature can break stuff.


Spoiler alert: this is not true for SE.

[bnemec]

There's an persistent and pernicious dogma in CAD (not just SW) that sheet metal parts must consist of only sheet metal features from the sheet metal app. Utter tosh!

Z-bends (including jogs) are a great reason to ditch this dogma. In many cases, it is far simpler and better for the design (you know, the thing that matter most) to control a z-bend in a profile sketch and use conventional features. Double-true if mount/contact faces are on opposite faces.

Conversion to sheet metal can occur after key features are created. This feature is there in every CAD package. The only reason not to use it is one's own self-imposed limitations. We have enough limitations imposed upon us without creating our own.

That's a bunch of rubbish. You are missing some use cases in your bold assumptions.

[HerrTick]

That's a bunch of rubbish. You are missing some use cases in your bold assumptions.

A boldness borne from nearly three decades of experience in multiple CAD packages in multiple fields.

Which particular cases would you say my assumptions are rubbish? I'll wait while you calm down and collect your thought.

[bnemec]

That brings us to another thorny problem with SWX. Converting to sheet metal destroys the existing body and replaces it with a new one. ("Old things are passed away; behold, all things are become new." If only SWX didn't take the Bible so seriously.)

Anyhow, the implications for this are huge. If you have ANY references such as mates dependent on that part geometry before converting it to sheet metal, they will break. Even reversing a jog direction and rebuilding the Convert feature can break stuff.


Spoiler alert: this is not true for SE.

@HerrTick This is the use case I was speaking of. Because of the product we deal with, consistent geometry IDs for the sake of assemblies are much more important than initial modeling speed. Assembly maintenance in all of the where used assemblies is one of the heaviest factors in how parts are modeled.

@mike miller It's not 100% true for Solid Edge, we've learned the hard way about a lot of things that screw up geometry/face IDs. Often times we would redo the revision edits to the model several times to identify which method disturbed the fewest assembly relationships. YMMV. There are certainly many of the wiz-bang modeling methods that are off limits in SE just because we've learned the future edits will likely ruin all the assemblies the part is used in. We rarely used the convert to sheet metal. Watch out for ST, it is rather flippant with geometry in our small observations. As I stated else where, we had become familiar with the minefields in SE. The minefields in SW seem to be similar but different.

[mike miller]

@mike miller It's not 100% true for Solid Edge, we've learned the hard way about a lot of things that screw up geometry/face IDs. Often times we would redo the revision edits to the model several times to identify which method disturbed the fewest assembly relationships. YMMV. There are certainly many of the wiz-bang modeling methods that are off limits in SE just because we've learned the future edits will likely ruin all the assemblies the part is used in. We rarely used the convert to sheet metal. Watch out for ST, it is rather flippant with geometry in our small observations. As I stated else where, we had become familiar with the minefields in SE. The minefields in SW seem to be similar but different.

@bnemec, I'd like to know the SE minefield in advance. Not too intimately, excuse the visual image.

[bnemec]

A boldness borne from nearly three decades of experience in multiple CAD packages in multiple fields.

Which particular cases would you say my assumptions are rubbish? I'll wait while you calm down and collect your thought.

Yeah, sorry if I came across brash; as you pointed out I need to calm down. I have several raw spots that have been open for nearly two years from this whole migration thing. We are into the thousands of hours of lost time redoing SW models due to poor planning and bad guidance from people who supposedly know CAD. @HerrTick You have not been one of those people.

[bnemec]

@bnemec, I'd like to know the SE minefield in advance. Not too intimately, excuse the visual image.

That's my point, unless I understand what your product and business practices demand of the CAD data I cannot give good advice to your specific application. Half of the problems we worked through may be mute points for you, and then we may have never used functionality that you might need so I'm completely ignorant of those mines. You'd wind up cussing me both ways!

[mike miller]

@mike miller It's not 100% true for Solid Edge, we've learned the hard way about a lot of things that screw up geometry/face IDs. Often times we would redo the revision edits to the model several times to identify which method disturbed the fewest assembly relationships. YMMV. There are certainly many of the wiz-bang modeling methods that are off limits in SE just because we've learned the future edits will likely ruin all the assemblies the part is used in. We rarely used the convert to sheet metal. Watch out for ST, it is rather flippant with geometry in our small observations. As I stated else where, we had become familiar with the minefields in SE. The minefields in SW seem to be similar but different.

Just did a quick test in SE. If you use the Thin Part to Synchronous Sheet Metal command, all is well and there will be no errors to downstream mates. The Part to Sheet Metal Command in Ordered swaps out bodies just like SWX.

So I was half right. Actually, since we use primarily Synch, I was mostly right.

[bnemec]

Just did a quick test in SE. If you use the Thin Part to Synchronous Sheet Metal command, all is well and there will be no errors to downstream mates. The Part to Sheet Metal Command in Ordered swaps out bodies just like SWX.

So I was half right. Actually, since we use primarily Synch, I was mostly right.

Converting to sheet metal builds a new body, I don't know of a case where it doesn't SW or SE (the redheaded step-sibling of NX). This wouldn't be the end of the world for us, we could still make the sheet metal part with convert as long as that is done before it is used in dozens of assemblies and prints. The problem I found is edits done later to features before the convert to sheet metal are very much more likely to change geometry IDs.

[jcapriotti]

I cannot figure out how to make a jog where the offset is less than the thickness, nothing I have tried is working and I'm out of ideas. I even looked at the help page, it was most generic on the topic.

Not as easy as Solid Edge but instead of a Jog you can use a Swept Flange and sketch the profile with the tangent arcs. Then link them to the thickness/radius values.

[bnemec]

How do I see all the variables for features? Can they be shown in the Equations. Global Variables and Dimensions dialog?

With a flat tab and an edge flange in both SW and SE this is what I get:

SW:

SE:

See how all the editable attributes of the feature can be edited from the Variable Table? In SW only dimensions placed by user are shown. When you want to edit stuff without going into the sketch or feature is this how you do it in SW? I used the variables table fairly often in SE.

[HerrTick]

Yeah, sorry if I came across brash; as you pointed out I need to calm down. I have several raw spots that have been open for nearly two years from this whole migration thing. We are into the thousands of hours of lost time redoing SW models due to poor planning and bad guidance from people who supposedly know CAD. @HerrTick You have not been one of those people.

I could have been kinder, as well.

You bring up an even bigger problem, one that transcends all CAD platforms: the collective base level of user skill. Way too many who can't see the forest for the trees.

There are way too many models that are a collection of near-random features that barely manage to turn into a useful object. I see so many users that are modeling but not designing. The smell of haphazard panic and desperation in some model trees is palpable.

"I may make you feel, but I can't make you think." --Ian Anderson (Jethro Tull)

It's a simple thing to teach someone how to make sketches and features. It is far more difficult to teach one to think about designs--how to think of and visualize shapes and how they interact with each other.

The "d" in "design" is for "planning".

[jcapriotti]

How do I see all the variables for features? Can they be shown in the Equations. Global Variables and Dimensions dialog?

With a flat tab and an edge flange in both SW and SE this is what I get:

SW:
image.png

SE:
image.png

See how all the editable attributes of the feature can be edited from the Variable Table? In SW only dimensions placed by user are shown. When you want to edit stuff without going into the sketch or feature is this how you do it in SW? I used the variables table fairly often in SE.

What you have selected (3rd button - dimensions) shows all of the variables for all features. I usually name them to make them easier to find.

SolidWorks only makes a global variable out of "Thickness" for some reason. So I double click the Sheetmetal feature to show it dimensions, and right click the radius dimension and select "Link Values" and call it "Radius". You can link other dimensions to it or use it in an equation.

The other things SE is showing appear to be items that are located in the Cut list in SWX.

[bnemec]

What you have selected (3rd button - dimensions) shows all of the variables for all features. I usually name them to make them easier to find.

I'm not following. "3rd button shows all of the variables for all features" it doesn't show the variables for the swept flange 1 feature (screen shot). It only shows sketch dims (twice for some reason) and a couple sheet metal object properties. I'm not seeing the properties/variables that are in the feature settings.

SolidWorks only makes a global variable out of "Thickness" for some reason. So I double click the Sheetmetal feature to show it dimensions, and right click the radius dimension and select "Link Values" and call it "Radius". You can link other dimensions to it or use it in an equation.

So to edit feature properties/variable (highlighted in screen shot) from variables table I need link them to global variables?

The other things SE is showing appear to be items that are located in the Cut list in SWX.

I'm still trying to figure out all the various things "Cut List" means... I assume it's more than a node in the Feature Tree, specifically the "Solid Bodies" node renamed when the fist sheet metal body is created?
from help;

A cut list is an item in the Feature Manager design tree that groups the same entities of a part together. It is available in parts that have weldment or sheet metal features.

If the parameters of features shown in the SE variables table are cut list items I'm totally lost.

[mike miller]

Cutlist properties are body specific file properties, if you will. For weldments and sheet metal, SWX will generate specific ones automatically( like thickness, radius, and reliefs). It's a little confusing, especially when the cutlist corrupts and you lose a bunch of data.

Here's a brief video that shows how to access it.

[jcapriotti]

I'm not following. "3rd button shows all of the variables for all features" it doesn't show the variables for the swept flange 1 feature (screen shot). It only shows sketch dims (twice for some reason) and a couple sheet metal object properties. I'm not seeing the properties/variables that are in the feature settings.
image.png

You won't see the dimensions for offset until it gets a value other than 0. Nor the radius dimension unless you uncheck "Use default" or "gauge table". Then the dimensions will show up. You can rename them from the default (D1) to something more useful like I did for the other. I wish SolidWorks would do this as a default. It does in some places like the hole wizard.

So to edit feature properties/variable (highlighted in screen shot) from variables table I need link them to global variables?

No, you can put them in as dimension equations only if you want. Thickness is a built in global variable, but not radius or K-Factor. If you plan to use them in equations I would create them as Global variables. Personally I like to do most all of my equations, at least the complex ones, as Global variables, then make the dimension value equal to it. That way I don't lose it if I delete the dimension or feature. I can also get the math and logic worked out before having it control the geometry.

I'm still trying to figure out all the various things "Cut List" means... I assume it's more than a node in the Feature Tree, specifically the "Solid Bodies" node renamed when the fist sheet metal body is created?
from help;
If the parameters of features shown in the SE variables table are cut list items I'm totally lost.

Cutlist properties are mostly read-only sheet-metal numbers, although you can manually add properties like raw material part numbers or descriptions. Then you can insert it into a drawing as a cutlist table.

[SPerman]

How do I see all the variables for features? Can they be shown in the Equations. Global Variables and Dimensions dialog?

If I recall correctly, NX had a sketch properties window. By selecting the sketch (not editing the sketch) the properties window would fill with all of the dimensions in the sketch. You could modify any dimension without editing the sketch, or going into a separate window (like manage equations.)

I can't find a great example, but this should give you an idea. In the screenshot below, anything you click on in the Part Navigator will populate the Details below. An extrude would have the properties of the extrude feature. A sketch would have all dimensions used in that sketch. It was a really efficient way to work.