Transitioning from NX 7.5, Advice? 3

[TylerCandela]

Solidworks Newbie..

Transitioning from NX 7.5 to Solidworks 2013

Everything seems counter intuitive, would appreciate any advice that might make this transition more fluid.

Thanks,

-Ty



Tyler Candela
CAD Operator
NX 7.5

 

[Eltron]

Run through the tutorials, hit up YouTube, and ask us a lot of questions.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[TheTick]

Be glad you're not transitioning to Pro/E, which is not just counterintuitive, but anti-intuitive.

Mostly SW is counterintuitive to NX users because your intuition has been conditioned to NX. First, stop reminding yourself how NX does things.

Any specific examples of what is vexing you? Or is this a general gripe/lament/wallow?

 

[TylerCandela]

Tick,

Everything seems very sketch dependent.

Modeling what should be a simple subtraction(a contoured part holder for instance) is farcical at best.

I guess that's a good starting point..



If you were to make a part holder from a block, how would you subtract the part from the block? I thought the INDENT command might be my savior.. but it doesn't function for me at the assembly level (where I would like to use it to subtract a part from an extruded block.


Also, I am wallowing hard. I feel like I've been sent to detail hell.

Thanks,

-Ty





Tyler Candela
CAD Operator
NX 7.5

 

[BiPolarMoment]

I rarely have a need to subtract a fully defined existing part from another part, so in most cases I would "cut" that material out of the block in one or more feature operations.

However, sometimes I have a need to make a perfectly form-fitting blocks (generally for FEA) and in those cases I do the following:

1) Open a "block" to subtract "part" from.
2) Insert Part "part" into "block" part (Insert>>Insert Part)
3) Use Move/Copy to locate "part" relative to "block"
4) Insert>>Features>>Combine>>Subtract (note: Combine is just a Boolean command)

Another option: You can model your "part" within the "block" document (or "block" within the "part" document) by deselecting "Merge Bodies" when you are creating features. Then you can "Combine" the parts as above.

I've always wondered why you cannot do a similar operation from an Assembly level but I think it has mostly to do with how the program differentiates between multi solid-body "parts" and multi-part assemblies.

 

[TheTick]

Insert --> Feature --> Combine --> Subtract

 

[TylerCandela]

Moment,

That's where I'm at currently. Accurately placing the tool part is quite difficult. Furthermore, once I've finally got it (a shcs) in place I cannot simply select the body of the screw without windowing over it, the points and curves can only be selected independently.

Also, the tool part is retained regardless of what options I choose in the indent prompt. Is there something that I am missing there?

Prompt -->

Result-->

Thanks,

-Ty

Tyler Candela
CAD Operator
NX 7.5

 

[TylerCandela]

If it isn't obvious the above pictures are just for example.

Tyler Candela
CAD Operator
NX 7.5

 

[CorBlimeyLimey]

Tyler,
You should be using the Combine tool, not the Indent tool.

 

[BiPolarMoment]

I'm not sure the Indent feature is what you want. As I and TheTick suggested I think what you want is Insert --> Feature --> Combine --> Subtract.

Then it will ask you which body is the one you want to subtract from the other and hopefully you get the result you desire.

 

[Updraft]

Tyler,

Since you are making a recess for a SHCS why don't you use the appropriate feature from Toolbox? It will size the hole and counterbore for you and even give you options to customize it.

It is evident you are an experienced modeler, just not familiar with SWX. I highly recommend you invest in the time to go through the tutorials as others have suggested. Help --> SolidWorks Tutorials. They are extremely well done and even give you an idea of how long it should take to go through the individual lessons.

For your particular problem of making a part with a cavity to perfectly match another part the advice above using Subtract is the way to go. You can read up on it in the SWX Help.

- - -Updraft

 

[TylerCandela]

Completely spaced earlier.

Combine --> Subtract is exactly what I needed.

Next time maybe I'll actually digest what I've read.

Reading up on tuts, just figured I'd hit the forum. (It had been incredibly useful when learning NX)

Thanks all.

-Ty

Tyler Candela
CAD Operator
NX 7.5

 

[TylerCandela]

Tyler Candela
CAD Operator
NX 7.5

 

[TheTick]

<zen>Be patient with yourself. You're replacing years of NX experience with hours of SW "familiarization". Don't be your own worst enemy. Be both patient teacher and willing student at the same time.</zen>

 

[frusso110]

I used SolidWorks in college (back in 2004-2008), then used I-deas and NX for my first job, and now am back to SolidWorks now. Could you please explain why you think everything is counter intuitive? I would be happy to assist.

 

[mjcole]

Tyler, Nice image i was writing as you'll see below a few comparisons and similarities differences between SW and NX.

As with most CAD systems SolidWorks can do most if not all the things that NX can. It will take a little while to figure out which of the numerous ways of accomplishing your task is the easiest and most robust. I'd suggest checking out the Shortcut Toolbar (S key default) Hitting this key or any other you assign brings up a mode sensitive toolbar Part, Assembly, Sketch, Drawing where you can assign commonly used commands to free up screen real estate and cut down on icons. Another good thing is it provides a simple method for accessing Customize Screen dialog other than the options flyout or selecting Tools pull down menu. Gesture support is pretty robust as well but if you are a strict toolbar man that's okay too.

Command Manager

Similarities of SW (SolidWorks) to NX.
1. MultiBody Modeling (Uncheck MergeResult in Protrusion feature Extrude, Revolve, Sweep, Loft)
2. Sketcher Relations dialog (Display/Delete Relations)
Display/Delete is not as robust as NX's one filter wise but dangling dimensions (Dims with missing references) are way easier to attach in SolidWorks. I hated how dimensions kept turning purple in NX due to this

Things you will miss if you haven't already.
1. Toggling sketcher dimension display: This is only possible for 3d Dimensions (check the View glasses in HUD) HUD is Heads Up Display the mini toolbar at top of display area.
2. Layers > These can only be used in Drawings, SolidWorks does not believe in using Layers for modeling/assembly modes.
3. Being able to continue a feature operation even in Hidden Mode or Hide Show a tree item.
I remember doing this in NX but in SW the bodies you are working on need to be visible.
4. Selection Box where you can select features, bodies, entities by color name or other identifiers as in NX

I used to work for a SolidWorks VAR and was always eager to speak with the former ProE & UGNX users because I knew specifically the functionality they were seeking and could ask them what they were doing before and guide them to the matching functionality in SolidWorks.

Further Notes
Combine command at Assembly Level is called Cavity. I'm not sure if you ever used the Wave Geometry on NX but I remember it being great though not active by default.

The Insert Part has two options
Translate/Rotate: Distances and Angles used to place body (Non Parametric).
Constraints: Add Distance, Parallel, Mate, Align constraints similar to assembly mates but controlled by part dimensions.

Read up on the 2013 What's New document from SolidWorks it can help you focus on newer functionality that will be replacing old functionality and might put you ahead of some of the SolidWorks gurus at your company who may be hardened in their Olde School modeling norms.

I do not believe that SolidWorks has Promote Body type commands as used in NX but I always found those added way to many steps to a simple process.



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Boston, MA
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[swdesigner]

Tyler,
Follow the advice above!!!

get used to customizing Solidworks it will help a lot.
The main thing I customize is the "S" key, saves a ton of time and mouse travel,
you can customize it in sheetmetal, part, assembly, drawing and sketch. Each one will
be a little different but once you have it setup it will help you sail thru SW.

Frank

 

[GRF]

My company does a lot of over molding so we run into this type of situation all the time. We use the Insert\Mold\Cavity command while editing the part in the final assembly. It removes the material of the parts selected that occupy the same space as the part you are editing. It also links the part to the assembly so you are not able to run a cavity command on the part in another assembly. If any of the parts that affect the "cavity" the cavity will be updated the next time you open the top level assembly. This is good and bad. It means if you use PDM and do not always have it loaded when you do it will almost always appear your local version does not match the version in the vault even if you have not changed anything. It does this because the feature is regenerated every time the assembly is opened so it appears the part has changed and you will be asked to save. The solution to this is to break the external references in the part with the Cavity. This will lock the cavity shape, but it will no longer update if you change the shape of any of the other parts.

You can also scale the cavity if needed. I am pretty sure this is the process that mold makers use when designing the mold for a injection molded or die cast part.

The icon "Indent" looks very similar to the icon for "Forming Tool". It makes me think that the material will be deformed around the reference shape. I could be biased though because I have used the Forming Tool often in another life.