Converting from AMD to Solid Edge - Basic Questions 3

[Prospero999]

Hi chaps,

I'm new here. I've used Autodesk Mechanical Desktop for many years, but am having to convert to Solid Edge ST1 as that's what my University wants me to do! Grumble! It's all very annoying!

I just want to ask a few basic questions to get me started:

1) Autodesk MD allows one to define not only work planes, but also work axes. Does Solid Edge allow work axes?

2) Autodesk MD allows one to draw a sketch and THEN choose whether one wants to extrude / revolve it, or whatever. Does Solid Edge reverse this - i.e. you define an extrusion and only THEN do the sketch?

3) Can I make 'floating' menus like in MD?

And that's it for now. I'd be most grateful if someone could give me a little guidance. It will go a long way!

Cheers,

Anthony

 

[beachcomber]

Q1. As I haven't used MD I don't relly understand what you mean by work-planes. In SE you can create planes by several means .... coincident, parallel, tangential etc.
You can then use these planes to create sketches, intersection curves etc.

Q2. Yes you can do it like this if it feels more familiar, but you don't have to.

Q3. This depends which version you will be using. Up to and including V20 you could do this, but ST versions use the Microsoft Office style interface, so you can only customise the Quick Access Toolbar.

SE is quite flexible in it's approach - you can create a plane, create a sketch on it then use that sketch to create a feature. This will give you 3 items in the feature tree.
OR you can go straight to the sketch command. The first step will then be to define a plane for the sketch. Once you have done this you create the feature. This will give you 2 items in the tree.
OR you can just select the feature type you want to create.
The first step will be to define the plane for the sketch, then you will draw the sketch and finally create the feature. This will create 1 item in the tree.

I am assuming here that you will be using 'traditional' mode. I haven't really used 'Synchronous mode' but things will be a little different if you do.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

Where would we be without sat-nav?

 

[PatCouture]

Hi Prospero999!

Welcome to Solid Edge! I worked with MDT6 a while back so I may be able to help you quite a bit.

Having to work with a new software is though and it will be a pain the first few weeks because all you'll want to do is to use SE with the same workflow as you are used to with MDT. My advice is be as open minded as possible to new ways of accomplishing things and don't settle to one way of doing your modeling, most of the times there are two or three different workflows that leads to the same end result.

First and foremost in the ST1 release of solid edge you have two completely different software available: a traditionnal parametric software (similar to MDT) and the new Synchronous technology which doesn't depend on a feature tree. So for us to help you best we need to know which one you will be using.

If you don't know which one to use right now it's alright. They are both useful and they have their own strength and weaknesses.

Right now I consider synchronous technology to be a great tool for imported geometry or to work with simple cubic shaped parts. But it's still a very young software. Traditionnal solid edge on the other end is a very mature product (more than 20 releases) with a lot more to offer. I think you will find yourself more comfortable with SE Trad because as I said it's the one who ressemble the most to MDT.

As for your questions:

Q1: (Trad) As beachcomber said you can define planes but there are no work axis in SE most of the times for your revolved feature you can use existing geometry for work axis. Or if you don't have any geometry to use you simply draw a line and you use it as a work axis.

Q1: (ST) You can also create planes but ST will lead you into drawing directly onto the model surface.

Q2: (Trad) SE can work in both manners but if you plan on using the sketches for other things you will need to draw it first. If you select the protrusion or cutout of whatever and draw the sketch inside of the feature, the feature will keep the sketch only for herself. you will be able to edit it later, but you won't be able to use if for other features.

Q2: (ST) You always draw the geometry first, then you select the proper feature to work with.

Q3: No! Your only hope lies in the Quick access toolbar but it's of little use with ST1

Good luck!

Patrick

 

[beachcomber]

I think if you are used to creating a plane, then a sketch, then the feature there is no reason not to carry on working this way.
All it means is more items in the feature tree.

Sorry I forgot about axes, but if you are creating a revolved feature just add the axis as a line in the sketch.

When you do start to use SE I would suggest going through some of the tutorials.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

Where would we be without sat-nav?

 

[burhop]

You might also hint to your university to go to ST2. It has a lot more functionality (synchronous sheetmetal, FEA) and improves on many of the things that were new in ST1.

My son is in the same boat with his university not upgrading :-(

Mark

 

[donyoung]

> Q1: (ST) You can also create planes but ST will lead you into drawing
directly onto the model surface

not quite correct. SE will create a local plane on that surface. The
one that you manually define is a global plane which can be referenced
by any feature you create.

======
ST2 has indeed some new functionality but unfortunately most
if not all can be found within the synchronous part of SE
only not within the traditional part. Sync-SheetMetal -- hmm, still
in Beta and will be implemented by a MaintenancePack (MP)
FEA -- hmm only available by a separate license (Simulation).
The bundled one (Classic version of SE) is still the same
only the name has changed 'SimulationExpress' ...

dy

 

[burhop]

I'm just talking academic version. Solid Edge Simulation comes with that so if you are at a school it's free. Plus the ribbon and quick access tool bar are both better in ST2, sketch performance is better, draft is better and it supports Windows 7.

Mark

 

[Gemnoc]

Hello Prospero999!

As one whose first parametric modeller was Mechanical Desktop 1.0 back in 1998, I can tell you that even with Solid Edge ST1's shortcomings (the ribbon bar, lack of toolbar customization, no work axes), I'd prefer a bullet in the head than going back to MDT!!! If you're doing 2D drawings, you'll see that SE's drafting module is much easier and faster to work with. Overall, performance is better, visualization of models is better.

Give it some time, try it with an open mind, and don't hesitate to come back here and ask questions, folks here are great!

 

[beachcomber]

Just so I can get an idea of what Anthony is coming from, could someone explain what a work axis is and why you would need one?

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

Where would we be without sat-nav?

 

[Prospero999]

Hi Beachcomber,

A work axis is simply a work feature like a work plane. It provides one with a reference around which one can perform a revolve procedure. One can define them in many ways. A couple of examples would be:

1) By selecting a couple of intersecting planes. Where they intersect, a work axis will be created.

2) Selecting the ends of a concentric feature like a hole. A work axis will then be created down the centre of the hole.

Hope this makes it clearer,

Anthony

 

[Prospero999]

Hi chaps,

One further question:

If one cannot define a work axis, one has to define a line to do the same thing. How do I define this line parametrically? I.e. so that it's locked into a fully constrained system?

This confuses me!

Anthony

 

[karmoh]

From the help system

Step 1. On the Home tab?Solids group, click one of the following buttons.
• Revolve
• Revolved Cut

Step 2. Do one of the following:
• If you want to draw a profile, select a planar face or reference plane.
• If you want to select a profile from an existing sketch, on the command bar, on the Create-From Options list, click the Select From Sketch option. This option is not available if there are no sketches in the document.

Step 3. Draw or select a profile and define an axis of rotation. The profile can be open or closed.

 

[beachcomber]

If you use an open profile the added material must fully join to the existing solid. Thus an open profile would not be valid for the first feature.

As for parametrically defining the axis, it's just a line in the sketch/profile of the feature. You would constrain it to existing geometry as normal.


bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

Where would we be without sat-nav?

 

[PatCouture]

Hi Propero999

To define the line parametrically, you should learn about the include command. It enables to include geometries from your part into a sketch (assuming your working in a part) or even including geometries from other parts in the context of an assembly.

Be carefull though I've been burn a couple of times with this features because I didn't know how to used it properly.

I don't know if this feature works for the Synchronous environment.

Hope it helps

Patrick