Are there any resources that map the functions I'm more familiar with in SolidWorks and Alibre Design to what they correspond to in SE? Perhaps a PDF explaining the mappings to someone coming from these CAD systems? I expect I'm not the only potential client who's never learned AutoCAD.
For example, I've gathered that "Configurations" of parts & assemblies are supported, but under the name "Families" of parts & assemblies. I spent quite a while figuring this out, and I'm eager to expedite the process as much as possible for the other concepts I'll need/want to get through quickly.
I'm aware that there's a "Command Finder", which is a good idea as far as it goes, but this found nothing for me when I looked for configurations, while the help system didn't offer me anything helpful either. It looks to me like this only covers how the AutoCAD commands translate.
Now I'm trying to understand where reference lines in sketches went to. I understand the concept that the history-based features are not the only game any more, but I was led to believe that SE offered robust support for both traditional features as well as the new synchronous way of doing things. When an engineering sketch can substitute for hours of analytical math, I expect I'll still need/want to use it as the basis for my part geometry, and many/most of the lines in such a sketch won't correspond to actual part curves.
Also, any tips for how to model a parabolic curve? This was a supported command in SW.
Any suggestions, links, or whatever you can offer would be welcome.
We deliver a "cross reference" tool in Solid Edge, it's called that Command Finder and lives at the bottom of the Solid Edge main window.
It's intended to help you find Solid Edge commands but we put a cross reference table with command names used in other system. Type in "Shell" and a small dialog will appear listing our equivalent "Thinwall" command. Hover over the found command it it will highlight where it lives in the Solid Edge interface.
I appreciate your response, but I guess you didn't see the part of my message where I'd said I was already aware of the command finder. The frustration is that this tool seems to know nothing about SolidWorks terminology (per my example, at least), and I know nothing about the AutoCad terminology. It's like being offered a russian-chinese dictionary when visiting Russia, but having no familiarity with Chinese! I like the concept of including such a dictionary, but it really needs to be relevant to the terms I'm familiar with, or it's useless to me. Is there anything or anyone else who could help me understand the points I've raised? I'm still not understanding where reference lines went to, or how to generate them if they're in there somewhere. The greater issue is that I'm still needing robust support for engineering sketches, which can sometimes get a bit complex, to save me from hours of mathematics. At this point I've got one sketch that worked immediately in Alibre Design, but which I can't yet get to work in Solid Edge. I'm aware of many other limitation of AD, which is why I'm considering SE, but I'd been hoping the premium cost of SE (compared to AD, at least) would come with premium abilities, outshining AD in every way. I'm sincerely trying to understand how SE really compares to AD and SW, and any help you or others can give would be appreciated.
I was connected to a member of the support staff at Siemens. She tried to phone me and that didn't work, because my business and phone are in the US, but I'm presently in India on an extended business trip. She sent me her e-mail on Feb 28th. Because of power and internet connectivity problems, I was unable to send my response to her until today, Mar 2nd. When I sent that email to her address from mine, I received the following email rejection notice:
"Your message wasn't delivered due to a permission or security issue. It may have been rejected by a moderator, the address may only accept e-mail from certain senders, or another restriction may be preventing delivery."
I'm therefore posting the response I'd attempted to send her, since I see no other immediate means of communicating this.
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Thanks for your response, and your attempt to call me.
The phone is my valid US cell phone number, but you didn't reach me because I'm currently on a business trip within India. You can reach me at +91-735-000-4561, although with the time zone differences it's probably easier via e-mail. If I remember correctly, the "+" translates to "0011" to reach the international circuits from within the US.
This is the first email I've written to Siemens, so I presume you're referring to my requests for help on the user forum. I'm including a pdf of the forum thread I created within the attached zipped folder in case that saves you some time. Unfortunately no one in the forum has been able to help me as yet.
I could still really use a reference document which mapped commands, functions and /or concepts from their SolidWorks names to the terminology used within SE.
In my last comment I referred to an engineering sketch from Alibre Design which I've not been able to replicate in SE. I've included a jpg of this sketch, so you can see what I was trying to do. The reference lines in AD are the dotted lines; while the lines that will turn into actual part geometry are solid. The same conventions are used also in SolidWorks. I'm still wondering what people do rather than using reference lines within SE.
The error I came up against when I tried to replicate this sketch was: "The requested change conflicts with existing relationships". I've attached my best attempt to replicate the sketch within the file "core_synch.par". In this file I got all the way to the last relationship before getting this error, and the relationship I was trying to add was to set the distance from the rightmost circle to the edge equal to the half distance between the inner circles, which describe where holes will go. I don't see how the new relationship conflicts with any of the existing relationships. It's the same sketch as in AD, so perhaps the relationship solver is just getting stuck. Or perhaps I made a mistake somewhere, although I certainly did my best.
This has been a frustrating error message; it seems that once I get it, I can never move forward in that sketch again, no matter how many relationships I eliminate. My only recourse has been to start over in a new sketch. I sincerely hope that I'm missing something in this; but naturally as a newbie I don't see it. To give you a concrete example, take a look at the file "core_stuck.par". Clearly I didn't get the relationships quite right, although the geometry looked much cleaner before I applied the relationships. Clearly the upper left corner of the triangle is not connected to the center of the upper left circle, so I tried to connect them, and got this same error message. Since then I've eliminated many of the relationships, but it still refuses to let me do anything that would move that upper left circle.
More recently I've been able to dramatically simplify the example sketch, as you'll see in the file "core_simpler.par". Within that file I was able to create a simpler and better-generalized example of my basic part design which worked. I was also able to manually adjust the hole to edge distance, and see how the hole to hole distances varied in response. That all worked very well, for a while.
Then I came across and worked through the tutorial on the Goal Seek command, and tried to apply it to the geometry in this file. This kind of ability goes beyond what's in Alibre, so I was eager to put it to work. I created a new variable, "Hole_Edge_Dist_Ratio", and tried to get the Goal Seek command to bring that ratio to 2.0 by modifying my hole to edge distance. SE let me define everything, but the Goal Seek command was unable to do anything in this case. It looked like it was diligently working on things, and spent over 20 seconds of calculation time on it, but didn't end up varying anything that I could see. Worse, now that I've added all this, SE will no longer allow me to manually modify the hole to edge distance. Solid Edge even crashed once, as I simply tried to vary this value, but within the variable table rather than where the measurement was, which didn't work. Now when I try to manually change this value I'm getting the error message: "The dimension could not be changed. The requested value conflicts with existing relationships."
I've tried deleting the ratio variable, but a new variable pops up, and I still get this error.
In summary of my current dilemmas, I'm not understanding why the Goal Seek command wasn't working in this case. If it can't be made to work, for whatever reason, then I'm not understanding what to do to get the sketch back to a place where I can at least manually adjust it again.
If you or any of your colleagues can lend me any assistance with this, it would be appreciated. I'm pretty sure that I can regenerate the whole part from scratch again, but I'd rather not waste my time on that if it can be avoided. I'm evaluating Solid Edge in the hope that it will be able to save me a lot of time. If I have to re-generate parts from scratch, it certainly won't be saving me time.
Seems like quite a few things to sort out here, between your specific issue and your eval process. Let's start first with your sketch... It would be helpful for you to explain what you are trying to do. Based on your description and the files, it appears the approach you are taking is overly complex -- but perhaps I am just not understanding the goal. That is, if you define the size of the hole and you define the distance of its edge to the edge of the plate, then you have fully defined its center location and all the rest of it doesn't make much difference -- just pattern the hole 3 times in a circle and you are done. Clearly, there is more to it than this. So what exactly are you trying to do -- what is the requirement of the design? Is the size of the plate unknown and needs solving? As far as your eval, please email me directly at firstname.lastname@example.org and I will try to figure out what is up. I need the following information: 1. Your full name and company name. 2. The state in the US where your company is normally located. 3. Where do you intend to purchase the software -- in the US? 4. Would you be purchasing while abroad or after your return - -when would that be. I will make sure you get the contact/help you need to fully understand the software. Finally, if you can send me a list of things you searched for with your SolidWorks background but did not find in Command Finder, that would be very helpful. We see lots of interest from SolidWorks folks and we'd like to flesh out command finder as much as possible. Thanks, Dan
Daniel and I are in contact offline and will figure out who can help him out on a more regular basis. However, I thought the following tips/video I provided might be useful to others as well. The goal in this case is to have the "meat" between the holes to be twice the meat that is between the edge of the hole and the edge of the part. Here are some tips when doing this that you will see in the vid...
1. As your sketch develops, try editing/dragging along the way to make sure its behaving the way you expect. That way you find out before you box yourself into a corner. 2. I am holding down the Ctrl key and using the scroll wheel on my mouse to change the dim values -- obviously you can't see that in video. 3. The fastest way to make a formula between dimensions is to double click on the dimension (not its text) and that will bring up the formula bar. That is what I do herein. 4. I use the polygon command, which saves you having to do a few constraints. However, notice that you really don't need a very complex system for this. 5. To do the tangent dimension between the circles -- pick the button for that within the dim command as shown in the video. 6. When you get it all done, you will want to switch to Ordered (RMB Transition to Ordered) to make the actual solid. Because this is a sketch driven feature with formulas like this, you will want to do that in ordered. http://screencast.com/t/NrHD23TZB
A little more on this. Apparently the final goal is to drive the outer dia to a particular value while keeping one internal dim to be 1.75 of the other internal dim. This is easily done with a function unique to Solid Edge (and Excel!) called Goal Seek. Here is a video of it in action on this part. There are more videos of how to use it on engineering problems at www.solidedge.com. http://screencast.com/t/BsYnzX1jda