Solid Edge ST9 Part Modeling

by MLombard on ‎05-31-2016 08:28 PM (3,385 Views)

This is the part of What’s New that I really get most excited about. There is a lot of new stuff to talk about with ST9. Let’s just jump in.

 

Display Ordered Model In Sync (hybrid display)

This one is for people who work in mixed sync/ordered modes. The gist of the idea is that you can show your ordered features while working in sync mode.

 

Here is a model I made in mixed mode. The sketches were done in sync, and the lofts were done in ordered. I can be working in Synchronous mode, select a sketch, move it with the Steering Wheel, and watch it update the Ordered features.

st9parts1.png

Of course you have always been able to do the reverse, working in Ordered, you can move your Synchronous sketches. My example would probably be better to change the length of the first Protrusion, and watch all the lofts update.

 

There are a couple of settings that allow all of this to happen. Solid Edge Options > General > Recompute Ordered Part After Synchronous Edit is a new setting, and is turned on by default. But you need another setting to make this happen. In Synchronous mode, right click on the Synchronous header in the PathFinder, expand Show All, and select Ordered Body.

 

Anyway, this is good news for people who have integrated Synchronous tools into your workflows.

 

Associative Mirror in Sync Part

st9part2.png

Another sync/ordered type of enhancement that you will find in ST9 is the ability to “Persist Mirror Associativity”. Synchronous Technology removes a lot of associativity from your modeling. And this is great, most of the time. Sometimes, however, you do need a little associativity. And the Mirror feature is often one of those times. So Solid Edge has added an option to persist the mirror associativity. Remember the terminology for remembering face relations is also “persist”. This means changes of this sort will not rely on the Design Intent settings to drive changes to mirrored (or symmetric) features.

 

st9part3.png

Via the right mouse button menu, you can also break the associativity, so that the Persist condition can be removed from mirrored geometry.

 

Offset Design Intent

There is now an addition to the Design Intent options called Offset. This will maintain the offset (parallel at a distance) for thin features such as ribs during a synchronous edit. In the past you had to apply a dimension to get this sort of behavior, now it will maintain thickness without a PMI dimension.

 

st9part4.png

Multi-Body Features

Multi-body workflows can be very powerful for various types of design. Master model type work is one such type. This is where you create an assembly as a single part, saving sections of the part out to create individual parts that come back together as an assembly. This is done in many cases to simplify in-context relations. Getting into the how and why about multi-bodies is something for a different article. Here I really just want to talk about what’s new in Solid Edge ST9.

 

You can select which bodies the cut applies to, which is a great addition to the multi-body tools for this release. This type of functionality affects extruded and revolved cuts, rounds, chamfers, ordered holes, and pattern/mirror of multi-body features.

 

st9part5.png

Solid Sweep

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Solid Sweep is a feature that enables you to simulate cuts with an end mill, or the space that a moving part will occupy. Sometimes sweeping a 2D cross section along a path does not give you the type of geometry that you are looking for. For example if you are trying to cut a lead screw into a rod.

 

st9part7.png

Just in case you were wondering, this is one of the applications of multi-body modeling.  You model the rod, and then as a separate body you model the end mill or cutter in its starting position. Then apply some sort of a path. In this case, a helix was used. The path must intersect the cutting tool.


This method is great for visually showing this sort of cut, or when you have to actually create the geometry in CAD because you have to do some sort of simulation or 3D print. To actually manufacture this part in steel, your shop would work from standard data rather than running toolpaths on this geometry.

 

Spiral Curve

st9part8.png

The Spiral Curve option is just another option on the Helix dialog. You still have to initiate it with an axis, but you can specify the spiral by a combination of any 2:

  • End diameter
  • Turns
  • Radial pitch

 

 

 

 

 

 

 

 

 

 

 

 

Point Support in 3D Sketch

st9part9.png

3D sketch is one of those tools that I think gets underused in Solid Edge. 3D sketches can be used as all-around problem solvers when you have geometry you need to figure it out, and you can do it by hand calculations, sometimes it’s just easier to let the geometry figure itself out.

 

Points in 3D sketch do a great job of providing a reference that is not the origin or another coordinate system. They also keep track of virtual intersections between lines when rounds are involved. 

 

I’ve used 3D sketch points in the past to mark where a light beam touches a surface, or use 3 of them to define a plane.

 

This feature is also evidence that Solid Edge is willing to revisit even a new feature and add to it when it makes sense. The 3D sketch itself is rather new in Solid Edge. As soon as it became available, one of the things people were asking for immediately was the 3D sketch point. And now we have it.

 

Material Table

The Material Table can now be displayed in three different ways: Library, Group, or Material display, sorted in ascending or descending order.

st9part10.png

st9part11.png

Also, when properties in the library do not match the part (called out-of-date), the properties will be flagged.

 

Assigning a material to a part will optionally color the part to the face style defined in the Material Table.

 

(It sounds like Solid Edge is becoming more conscious of the display and appearance of models…)

 

Material properties are created as variables and can be exposed as file properties. Start imagining now how you are going to make use of this.

 

Summary

I’ve got to leave a little excitement for later. These are some pretty good enhancements, and it’s hard to believe how much they squeezed into this release. With all of the Data Management stuff, it’s amazing that they were able to do anything else at all.

 

Comments
by Legend
on ‎06-01-2016 02:44 AM

Matt, I've yet to see anything (the little bit I've read) about sketch relationship colors being added to 3D sketching?

by MLombard
on ‎06-01-2016 09:36 AM

@Craig_H no, if it's there, I can't find it. Meaning the functionality or any mention of it.

by Creator
‎06-01-2016 09:37 AM - edited ‎06-01-2016 09:38 AM
This method is great for visually showing this sort of cut, or when you have to actually create the geometry in CAD because you have to do some sort of simulation or 3D print. To actually manufacture this part in steel, your shop would work from standard data rather than running toolpaths on this geometry.


Why would the machine shop not use the geometry created to make the toolpath? This has been one of our frustrations is that it's time consuming to make accurate geometry for use in the rotary axis of a CNC mill, but it's even more time consuming to try to get the CAM package to make the most efficient toolpath you want consistently.

To the extreme where I've had to use MasterCAM to unroll chain geometry tool path it as a 2D path, then axis substitution it as the toolpath for use in the rotary axis. Simple 3 axis toolpaths are very easy to toolpath extremely efficiently consistently, when it comes to multi-axis roughing and machining it becomes increasingly difficult to be efficient and even more difficult for it to be consistent often just changing a feed or speed can mark an operation dirty and make it have to be regenerated and you end up with a completely different path the second time.

Being able to just chain the geometry right from the model and know it will be correct is a huge asset.

I used MasterCAM for the unroll function, because this is something that I haven't found solid edge to do easily, nor effectively, another frustration when you're trying to flat pattern solid bodies that are not sheet metal.

 

by MLombard
on ‎06-01-2016 10:43 AM

@sunderlandjoeOk, I'm not a machinist, but... The reason you wouldn't use the geometry cut by the Solid Sweep is because of the approximations involved. The software is approximating the cross section in the direction of the path. This can lead to some small imperfections in the surface that would cause problems in an application where you need surfaces to be highly polished.

 

Think of the process of knurling. You can create knurled geometry in CAD, but you wouldn't lay down a toolpath on that geometry. You set up your lathe with a knurl roller, and use that process to create the geometry.

 

Same with threads. You either roll the thread, tap it, cut it on a lathe, but you wouldn't just throw it into a mill with a 3D toolpath. You don't cut threads the same way you would cut a decorative surface.

 

Does that make sense?

by Creator
on ‎06-01-2016 10:57 AM

@MLombard


Yes, that makes sense.

if that approximation is reasonably accurate a lot of times that's all that's necessary.

You typically will want to rough out the bulk of the material as fast and efficiently as possible so if there's small errors that's completely fine at high enough feeds the machine wont even be accurate, it will cut corners, and there's tool deflection and many other dynamics at play.

However I completely disagree with the notion that the software cannot or should not be making the geometry accurately, as a machinist when I am sent a model, they get the part to the model, I use the geometry the CAD software is creating and use offsets on the machine tool to make it dimensionally correct. It is not reasonable to expect the machinist to be an engineer. They will not be able to create correct geometry in the CAM software it's very cumbersome and time consuming, the machine shop will not be able to make money this way.  

A lot of times if they're not sent the model, they will be creating the geometry as best they can with the CAM software which will make the same and more often then not worse errors.

For the lathe then yeah, it's very easy to make the turning profile, and use threading tools ground to the proper thread profile, and use a knurling tool for cosmetic geometry as you won't be chaining each helix for a thread, or line for the knurl.

For milling this isn't the way it works, which is what this tool seems to be intended for. If you're making a helical slot for a pin to ride in for a winch or something like that then the geometry in the model had better be correct because that is almost definitely what the machine shop will be producing it too. This is the advantage of having CAD/CAM software, if you have to manually draw lines for everything parts become expensive, being able to import a model and chain the geometry to make a proper part is necessary.

This tool brings in the huge advantage for 4 axis milling, as without having the fifth axis a lot of time making the "swarf toolpath" makes incorrect geometry because it's impossible to make the compound angle to a surface without being able to tilt the part.

by MLombard
on ‎06-01-2016 12:08 PM

@sunderlandjoe Don't get the wrong idea. I'm not talking about complex shapes in general. I'm talking specifically about 3D sweep and high precision process-based machining. If you have to manufacture some irregular cam profile, you have to work from the geometry. It's just that the cutter cross section is created by approximating a 2d shape, and then the 3D cut is made by moving that shape to discreet points along a path, interpolating between the discreet points. So that's a compound approximation. You wouldn't want a .5mm sized wiggle on a high speed cam path. Other software I've worked with worked the same way. I'd just recommend making sure the resulting geometry fits what you need to do with it.

by Legend
on ‎06-01-2016 04:31 PM

As long as this topic is totally hijacked, could you rough cut based on the solid and then profile the finish cut from a sketch? I do CAMWorks, but I'm not licensed for 4th axis, so I'm just guessing. Of course you probably lose the sketch in most CAM software.

by MLombard
on ‎06-01-2016 05:56 PM

@lking Yeah, you could rough cut to anything that didn't gouge.

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