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Feedback after a year of Pro usage
Ben_Misegades
Member Posts: 133 ✭✭✭
As is implied by the title, I've been using Onshape "Pro" for a year now, with a pretty good amount of time prior to that as a free user.
There have been a lot of highly valuable additions over this time span which is making Onshape more and more usable for my work, such as the addition of sheetmetal and now finally sheetmetal with large radii i.e. tubes and stuff. Weld symbols in drawings is another valuable addition, plus many more.
I'm a huge advocate of Onshape and recommend it highly to everyone. That does not mean that I think Onshape is perfect, though. As a matter of fact, after having used Onshape for this long now, in my eyes there are some glaring deficiencies:
- Lack of assembly-level sketches: this is something I've used a LOT in the past, but Onshape does not have them. I don't know how one would effectively make an assembly layout without it. Luckily my current line of work does not require much in the way of assemblies.
- Lack of planes in assemblies: again, something I used a LOT in the past, and in my eyes a must-have for any large-scale assemblies, yet Onshape does not offer it. Again, as luck would have it my current line of work can be done without them, with some irritation, but I don't know how people would manage large scale assemblies.
- Planes and sketches of parts are inserted into an assembly independently of their parts, and retain no apparent physical connection to them unless specifically stated. Mind-boggling.
- Mate connectors instead of mates: I find mate connectors to be infuriating and cumbersome. I've tried to give it time to allow myself to get used to them, but they strike me as being far less flexible in use than a traditional assembly mate. Furthermore, the fact that they're based off of part geometry is, in my eyes, a bad move as in evolving project design, geometry tends to change. I don't like my assembly "mates" to change if I start adjusting or even deleting geometry. This is why, in the past, parts or subassemblies mated into greater assemblies that I've worked on have been done using mates between planes almost exclusively, never part geometry.
- Assemblies: adding a new component to an assembly is frustrating as you can't easily move it, it just sits there rigidly. You also can't easily mate it as there are no planes to use or you have to screw around with mate connectors first.
There are more, but these are the top few that cause me unholy nerdrage on a regular basis.
There have been a lot of highly valuable additions over this time span which is making Onshape more and more usable for my work, such as the addition of sheetmetal and now finally sheetmetal with large radii i.e. tubes and stuff. Weld symbols in drawings is another valuable addition, plus many more.
I'm a huge advocate of Onshape and recommend it highly to everyone. That does not mean that I think Onshape is perfect, though. As a matter of fact, after having used Onshape for this long now, in my eyes there are some glaring deficiencies:
- Lack of assembly-level sketches: this is something I've used a LOT in the past, but Onshape does not have them. I don't know how one would effectively make an assembly layout without it. Luckily my current line of work does not require much in the way of assemblies.
- Lack of planes in assemblies: again, something I used a LOT in the past, and in my eyes a must-have for any large-scale assemblies, yet Onshape does not offer it. Again, as luck would have it my current line of work can be done without them, with some irritation, but I don't know how people would manage large scale assemblies.
- Planes and sketches of parts are inserted into an assembly independently of their parts, and retain no apparent physical connection to them unless specifically stated. Mind-boggling.
- Mate connectors instead of mates: I find mate connectors to be infuriating and cumbersome. I've tried to give it time to allow myself to get used to them, but they strike me as being far less flexible in use than a traditional assembly mate. Furthermore, the fact that they're based off of part geometry is, in my eyes, a bad move as in evolving project design, geometry tends to change. I don't like my assembly "mates" to change if I start adjusting or even deleting geometry. This is why, in the past, parts or subassemblies mated into greater assemblies that I've worked on have been done using mates between planes almost exclusively, never part geometry.
- Assemblies: adding a new component to an assembly is frustrating as you can't easily move it, it just sits there rigidly. You also can't easily mate it as there are no planes to use or you have to screw around with mate connectors first.
There are more, but these are the top few that cause me unholy nerdrage on a regular basis.
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Comments
Some of what you are pointing out is definitely a case of 'shame on us for not making this easier', and some simply a case of our intent not being more easily understood.
I would like to make you an offer!
Would you be willing to sit with me (virtually) for an hour with two goals in mind;
1) To learn from you what your expectations are.
2) An opportunity to show you how we thought the workflows would be used.
Perhaps if you chose to take me up, you might be inspired to post a follow up?
pthomas@onshape.com
Twitter: @onshapetricks & @babart1977
@Ben_Misegades : @philip_thomas has offered his time to go over workflows with you but in the mean time I would like to ask few more questions to understand details of pain points and also have some discussions going around these workflows.
- Have you tried using a part-studio with one sketch and inserting that sketch in assembly as layout? I understand it adds steps in editing the layout sketch and seeing the changes but are there other stumbling blocks in using that as layout?
- Our intention was that part studio mate connector and sketch will provide similar functionality as mating to planes. Did you try defining mate connectors in part studio and using that to mate parts? I can see issues in stability of part's identity itself if a part is changed drastically in multi part part studio environment but using part studio mate connector can help issues with changing geometry.
- We have internal discussions about bringing more than one part, sketches, surfaces and have them automatically become one rigid instance in assembly but for now they can be grouped after bringing in assembly. Will that be useful in your workflow?
@brucebartlett : There are lots of work planned in assembly area in near future. Can you provide some details of pain points in your workflow? I want to make sure we understand those and capture them for future work.
Thanks again for your feedback and I would love to hear more from you guys and others on these topics.
- Showing mates only related to specific assembly level not all below that level.
- Establishing free to move parts, not fully defined by mates. (fixed part icon a great start but we need more)
- Configurations, for me I have much more use for configuration/variants in assemblies than part studio's
- I love the idea of Positions but struggle to make them work and update with changes.
- Dragging mates in the tree to create groups
- Adding mates to folders
- Expand assembly tree by clicking a part in the view area. (I spend a lot of time expanding trees to find parts).
Malay, I am always happy to do a web call to show you my issues first hand. BruceTwitter: @onshapetricks & @babart1977
@Ben_Misegades Sorry if we digressed from original post a bit. I will be interested in understanding issues posted in your original post also. Those are all important topics so I would be happy to talk to you directly on them too or just continue discussing here in this thread whatever you prefer.
- I think you're right about being based off part geometry. But most of the time it is Ok. I will definitely take advantage of planes whenever that comes out! - I'm not sure what you mean you cannot easily move inserted parts... just click and drag ;p
- Don't forget you can select the mid point in a line while mating to act just like a plane. You don't need to create an actually connector unless you really want a coordinate system to mate to. It sounds like you are making a mate connector for each part before bringing them into the asm... Did I understand you right?
Let's see if I can answer this
- Yes, I can make a sketch in a part studio, then insert it into the assembly. This works relatively well, but seems like unnecessary steps. Again, I'm "spoiled" by what I was able to do for so many years in Solidworks.
- Yes, I've used part studio mate connectors along with sketches, etc. to attempt to help me position components in an assembly, but again, it seems like far too many steps for something that can be so simple.
- When I dump entities into an assembly from a part studio, I always have to group them to keep them together. Ideally this would have some sort of effect of components in the tree (like foldering) to keep it from becoming quickly overpopulated. I would rather see complete part studio insertion be treated as a "sub-assembly" in assemblies that are a single entity in the assembly tree with the option to explode or dissolve it into its constituent components. Separately, I'm rather perplexed by why a part inserted into an assembly can be done independently of the sketches it was made from.
- There have been a few instances where mate connectors have been more efficient as I may have to use one or two less "mates" than usual. However, there have also been instances where I find it to be next to impossible to mate a part into an assembly where I want it. It seems like mate connectors work well when there is definite geometry present upon which to base them, but if you don't have that things become very difficult.
- I learned the hard way in the past what happens when you base mates off of geometry too much.
- Now rotate them
- It is exceedingly common for me to want to use a coordinate system (or similar) when mating, rarely do I want to actually mate geometry to other geometry, such as face to face or similar as I have come to see this as a bad practice over the years. Perhaps I'm behind the times in my thinking, but any time I have anything other than a "simple" assembly, I prefer to mate all parts and sub-assemblies to a single, controlling entity such as a layout sketch or "base part" (composed of many sketches and planes). That way I can easily and quickly adjust my assembly and never worry about geometry changes/additions/deletions of my components affecting anything else in the assembly.
For a "simple" assembly, like I was working on yesterday, I'm content with making a few distance mates between planes in an assembly and the planes in the part I'm mating in.
I'm not saying that any of that is impossible in Onshape, but it certainly seems to be a fair amount more cumbersome to do.
Understanding desired workflows and a users interpretations (correct or otherwise) of functionality we write is critical to making Onshape better.
We actually agree with many of your points just based on your descriptions! That said, we would VERY much like to have you show us the mating situations you are struggling with. Myself, the assembly team leader and a representative from UX would all like to hear/see your pain/challenges.
Please reach out to us (pthomas@onshape.com) and let us know when would be a good time to show us.
If you don't, we will secretly connect your account to TinkerCAD with the openSCAD interface!
Philip.
Twitter: @onshapetricks & @babart1977
CAD Engineering Manager
Twitter: @onshapetricks & @babart1977
You can kind-of do that, as in this block mated using "SolidWorks-style" face-coincident, edge-coincident, and face-coincident mates instead of a single Fastened mate using OS-native mate connector style. At each step, pick any mate connector on the face or edge, and eventually constrain all DoF:
https://cad.onshape.com/documents/338c9dde0f9ffc90723982e0/w/fb75c15a9e5a5a2d96834a33/e/5566e996444eb074e7a96f6e
I find that the more I think in mate connectors and not in terms of SolidWorks mate types, the less I'm frustrated by them; I wouldn't call the above set of mates the correct way to connect these parts, and adding a (possibly floating w.r.t. the part) mate connector based on a sketch location helps in the more confusing cases.
The last time mate connectors got a thread in the forums, someone did bring up the point that while they streamline attaching parts, it's less easy to use them as a way of ensuring your parts are designed to properly control degrees of freedom - plane-on-plane or cylinder-coincident mates correspond to physical constraints in a way that mate connectors don't always.
PhD, Mechanical Engineering, Stanford University