Very painful switching from SolidWorks to Pro/E

[MichaelSW2Proe]

I recently switched from SW to Pro/E WF5, it is very painful. A lot of convenient things seem not available in Pro/E.

1. In SW, I can pick anywhere in an assembly, say an edge of a part, the part will be highlighed in the model tree on the left. In WF5, no way, it is difficult to do this backward matching, you can only pick in the model tree and see it highlighted in 3D model.

2. In SW, you can right click on a part or multiple parts/sub-assembly in an assembly, and choose "Isolate", it will isolate these parts and hide the rest. In WF5, no easy way to do this, you have to select the rest and hide.

3. In SW, you can right click on a part or multiple parts/sub-assembly in an assembly, and make these parts semi-transparent, very useful in observing a big assembly. I don't know how to do this in PTC, probably a lot of clicks needed.

4. In SW, when measure some dimensions, it is easily to switch the measuring units, no matter what is the part unit set up for, and it can show two units at a time i.e.(mm&in), in WF5, it only sohws one unit. I don't know how to show two or switch show in other unit for measuring.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[rohit_rajan]

2. in proe wf5 press Ctrl and select the parts you want to isolate then RMB and select Representation and select "Master"..it will isolate your parts exactly as in solidworks.

if you want to have your main assembly back look for "View manager" , in View manager under Simp Rep there would be "+" infront of master rep just doulble click on it, you will have your main assembly back.

and if you want to save the particular "isolation" just right click over the "+" sign and RMB save.

1. in wf5 also if you pick on the graphics windows it will surely highlight in the model tree and vice-versa.

3. to make parts semi transparent select "view manager ", select style, in bottom left you will see properties, select it then on the top you will see the option for transparency.

once you select the part the 3rd option is for transparency.

4. the changing of units while measuring i think is not there in wf5, but creo 2.0 has it now.

[MichaelSW2Proe]

Thanks for replying.

For 1, it seems only parts in the top level assembly works this way, if a part in a sub-assembly, nothing will happen, but in SW, no matter how deep a part is buried, it will be found in model tree, and highlighted, which is very convenient.

For 2,3, I will try tomorrow. Seems a lot more clicks than SW.

[rohit_rajan · Accepted solution]

there is one more option which would highlight the part no matter where it is deep inside ...

go to Tools> Customize Screen>View>One..select it and drag it to the toolbars somewhere..then select a part in the graphics window...and click on it..it will highlight in the model tree.

They are different Softwares...Michael..they will have there differences!

[MichaelSW2Proe]

This "one" button works fine. Thanks.

And the Isolate and Semi-Transparent things worked too, a few more clicks than SolidWorks though.

Now another unconvenient thing for me.

In SW, when you make sketch, you can make any existing geometry as reference and snap to that, if some geometry is hidden, just turn shaded view to wire frame and you can snap to that hidden geometry. That function I used everyday conveniently.

But in Pro/E, I cannot snap to those geometry by default, I have to create Sketch References first. That really slows down my design. Any way to make it like the way SW does?

[dschenken]

If you dimension to them or if you Use Edge, they are automatically added as references.

I believe if you use Align/Point On, they are automatically added as references when they are selected.

[MichaelSW2Proe]

The Use Edge function is another way of creating a Sketch Reference first in my understanding.

For example, on a rectagular surface, I need to draw a line from mid-point of an edge to mid-point of another edge in Sketch mode. In SW, you just draw a line, starting from mid-point of one edge to mid-point of the other edge, total two clicks. Done.

In Pro/E, you have to Use Edge to draw the two edges first, then draw the line, then delete the two edges you created, makes it more than triple time I needed in SW to draw a line. That sounds really stupid.

[dgschaefer]

In SW, edges are all you can use to align your sketches. In Creo, you can align sketch geometry to surfaces that are normal to your sketch as well. Surfaces are much more robust than edges and will produce a more robust model. Avoid aligning your sketch geometry to edges in Creo if a surface is available.

[MichaelSW2Proe]

Don't know what you are talking about. SW can use surfaces for sketch reference for sure. And in Sketch mode, all surfaces become lines.

[dgschaefer]

Not in my experience. If you spin a model in SW and try to align a sketched line to a planar surface, it won't let you select the surface. You have to select an edge. You can align to datum planes, but not model surfaces.

In Creo you can do either and using the surface is more robust.

[MichaelSW2Proe]

I tested in Pro/E about what you said using surface as reference but found out that you still have to convert that surface to a Sketch References first and all the Sketch References are all lines and curves eventually. While in SW, you don't need to do the first step to create Sketch References but just make sketch directly in reference to all existing geometry. In my opinion, the Sketch References step is a redundant step and makes Pro/E much slower in Sketching things than SW.

[StephenW]

Since I'm not sure exactly how SW works (haven't used it in years), Prior to selecting any references, the way I get a line to be on the midpoint (for the sake of this discussion) is to first sketch the line I want to start on the midpoint. Then I add the midpoint constraint. I think it's the least number of steps.

You will not get a one-to-one process for every thing you did in one software to the other. Pro/e will be more click intensive (learn to make and use mapkeys for repetitive operations). But don't give up searching for easier ways to do things in Pro/e. There are so many ways to do the same task. One will work better in one situation, other methods will prove more robust, and others will be more difficult/easy.

If you obsess over the all the little details of each operation, you'll never get your work done and you'll hate your job.

And if you haven't gotten to the drawing mode, hahaha, you are in for tons more pain.

Steve

[MichaelSW2Proe]

That's also what I figured "the least number of steps." to get a line to be on the midpoint, and it is more than triple of time to do it in Pro/E than SW. See pics below. Above pic is SW, it only takes 2 clicks to draw a line from 1 mid-point to another mid-point and it's fully defined (black, if not fully defined the line would be blue). in Pro/e, you have to draw two end edges first to create the Sketch References then draw the line, then delete the two initial lines.

I don't see how more robust can thse two extra end edges provide. If the shape changes, SW can adjust the line to the shape too. If the radiuses are gone, SW will remind you some reference is missing. This is just a simple example. Think about very complex geometry, how many more extra references you have to create in Pro/E?

[StephenW]

You don't actually have to draw the endlines (or use edge). You can just add the midpoint constraint to the endpoint of the line to the midpoint of the edge (has to be an edge, can't be a surface).

There are no more or no less references in your example from SW to Pro/e. You are referencing the 2 edges in both systems.

Pro/e is very explicit. It requires 100% definition. From what I remember about SW, it can be as loosie goosie as you want it to be. Great for concept, a potential catastrophe for production. But I suspect it all about being a good user, of which I was not one on SW.

Your specific example above is one of those no-no's in pro/e. You never want to reference the edge of a round. It'll haunt you.

Steve

[Inoram]

STEPHEN WILLIAMS2 wrote:

Your specific example above is one of those no-no's in pro/e. You never want to reference the edge of a round. It'll haunt you.

Steve

I think that's a no-no in any software.

[MichaelSW2Proe]

Thanks. That's a helpful answer, better than the method I metioned. Still 7 more clicks and a lot of mouse travel than SW (1 left click on the midpoint constrain, 1 right click for query select, 1 left click to select edge, 1 left click to select end point, then repeat 3 clicks on the other end).

That's just an example to describe the trouble, there could be more perfect example, and sometimes it's inevitable for this kind situations, i.e. to add feature to an imported dummy solids.

[rohit_rajan]

Michael...just want to remind you..because Pro/E is there..so Solidworks was able to simplify itself...eveything in solidworks is a copy of Pro/E....and made better.

Sorry i have to say this...but you keep talking about clicks and mouse travel...

try to use pro/e the pro/e way..otherwise you would always find issues with pro/e...

Solidworks was made to be easier to use..and they have done well..there is it where the comparison ends.

[dgschaefer]

Creo does ask you to select references prior to starting to sketch (unless it has been able to assume some), however you don't have to pick anything. You can close the dialog and start sketching. It will warn you that you haven't selected any or enough. It's fine to ignore it and start sketching. You will have to align your sketch to something before you can complete the sketch, however.

This goes back to the difference in philosophy I talked about earlier. Creio wants to you to tell it what references to use for this feature and it then limits its assumptions to those references. It is an extra step, but it goes back to the importance it puts on your reference selection.

However, you do not have to pick a reference ahead of time in order to use it. For example, I can create a dimension form a sketched line to a model surface without adding that surface as a reference first. I simply pick it during dim creation, Creo adds the ref for me.

Oh, and surface show in sketcher as lines because that's the 2D projection of the reference on the sketch plane. It does the same thing with a 3D curve or any geometry.

[dschenken]

If there is a sketch you think could be done more easily, post a screen grab and people can help with that.

No one here can change how Creo works, at least not for a couple of years, What you are asking for has been noted for at least a decade and nothing has seriously changed, except to make some things harder.

[JoshH]

Reminds me of the good 'ol days. Wonder how long it's been since a whitepaper was submitted.

[dschenken]

Have you ever built a Guillows flying model airplane kit and wondered how they got balsa wood denser than most oak? On a guillows board a guy wrote that he was going to send a scathing letter to Guillows about their terrible wood selection and how it made models that can't fly. Someone else then posted they'd seen a framed letter at Guillows that was a scathing letter about the terrible wood selection, proudly displayed in the front office.

Sometimes I imagine that PTC headquarters has a room paneled in layers built up of user submittals hoping that some improvment in the basic functions could happen. Very thick layers. Perhaps this year's User conference will get to see that room in a behind-the-scenes tour.

[dgschaefer]

You do not need to add refs first. If you select the constraint you want (coincident, parallel, etc), then the sketch entity you can select any appropriate geometry from the model to use.

Be aware, however, that how Creo & SW handle refs is different. SW is built around the idea of using whatever ref is convenient. If, upon rebuild, that ref is gone or not usable, the feature or sketch will fail and you can fairly easily redefine it to somethign else.

Creo is built around the idea of using the ref that matters and makes sense for what you are trying to accomplish. It will try to maintain those ref choices more tenaciously than SW will. If you are careful about what you choose, it works very well, allowing very robust models that respond well to changes. Casual ref selection will cause you trouble later as Creo tries to maintain those choices.

It's two different modeling philosophies, neither is superior to the other (though I certainly prefer the control I get in Creo), but understanding the difference will help you. If you drive Creo with the casual reference philosophy that SW rewards, you will be sorry. Conversely, if you try to build the kind of diligence into SW that Creo rewards, it won't matter much.

The point is, be very deliberate about what you choose as refs and Creo will reward you.

[Inoram]

Rohit Rajan wrote:

2. in proe wf5 press Ctrl and select the parts you want to isolate then RMB and select Representation and select "Master"..it will isolate your parts exactly as in solidworks.

if you want to have your main assembly back look for "View manager" , in View manager under Simp Rep there would be "+" infront of master rep just doulble click on it, you will have your main assembly back.

and if you want to save the particular "isolation" just right click over the "+" sign and RMB save.

I didn't realize this, I always wanted this feature. It works good, in creo2 it works on sub-assm parts, too so, not sure if the function is different then wf5. It would be nice if canceling it was slightly easier, though.

[jsarkar]

Mechanisms in sub assemblies are retained in PROE but not in solid works, check that. it will be treated as rigid in solid works

[ptc-5767400]

the right answer is to every 3d software has own exclusively advantages over other software,you mustn't find a better job which is with respect to Mechanical Desing or product stucture design if you can't be familiar with the PROE/CREO in ShenZhen City in China

[dschenken]

While not an option for Wildfire, apparently in Creo this has been improved:

from usecreo dot com/ten-new-capabilities-of-creo-parametric.html

8)Selecting Sketcher Reference “On The Fly”

Have you ever started sketching a profile and then realized you would like to snap the sketch to some underlying geometry? You can now add these references “on the fly” by holding the [CTRL] and [ALT] keys and selecting the edge, plane, vertex, etc.

[StephenW]

I just tried this tip...works like a charm in Creo 2. Now just to remember to use it as I am working. Not at all intuitive to hold CTRL+ALT but it does make adding the references easy.

[bp]

The bottomline: nothing great comes easy.

[doneill]

Great Thread... Thanks... Learned some good tricks!