SolidWorks VS Inventor

[corey_danielson]

I have used SolidWorks for the last 13 years. I have been using Inventor for the last 6 months. Before SolidWorks, I used PRO-E for 4 years (I had a seat of PRO-E at home for a side business, now I have a seat of SolidWorks at home for my side business. Just a little background to start with. I have noticed several items that I like much better with SolidWorks. But I figured this was a good place to try to get some answers. Am I wrong on any of these comparisons?

I might be, again I have only been using Inventor for 6 months. Please let me know if I am wrong on any of these, maybe I haven't done something correctly.  I am not bad-mouthing Inventor, I much prefer SolidWorks at this time.

I am willing to listen to any suggestions to my comparisons.   Thank you

[jtylerbc · Accepted solution]

I'm a little short on time, so I'm not going to respond to every point you make.  But I can touch on a few that are relatively quick to address, and maybe I'll get back to this thread later to address more.  A few of your complaints are valid.  Most are your own lack of knowledge, and a some are unclear what the grievance actually is (possibly due to my very limited familiarity with Solidworks).

• Pack And Go:  Hard to understand exactly what your complaint here is, because all you did is describe what Pack and Go in Inventor is supposed to do.  It it is not supposed to have anything to do with renaming files.  It consolidates a copy of the files to move them to another computer, send them to a supplier or customer, etc.  If you're having trouble putting a nail in the wall, it isn't the screwdriver's fault that it's bad at being a hammer.  It sounds like you should be using Design Assistant instead.
• Custom Properties:  Literally everything you listed in this point is incorrect.  You can do all of that in Inventor.  There may be some subtle points that Solidworks can handle better than Inventor - I don't know.  But everything you actually mentioned is possible.
• Maneuvering (3D Orbit):  I could make the alternate complaint that Solidworks makes it too difficult to pan because it put Orbit on the middle mouse instead.  This is a preference with no objective right or wrong answer.  Regardless of your preference, look at the "Display" tab in Application Options and change the "Middle Mouse Button" settings.  What you're complaining about are just the default settings, if you don't like them, change them.  
• Basic Commands (Zoom Extents):  In Inventor, you don't need a button for "Zoom Extents".  Double-click the middle mouse button.
• Extrusions within an assembly:  Not being a Solidworks user, I'm a little unclear what you're attempting to replicate here.  But if you don't want to open the part or subassembly, don't double-click it.  That's what double-clicking does, and there's no other reason to do it.
• Flexibility:  This can legitimately be tricky to use in Inventor.  Would need to see an example of what you're trying to do to figure out exactly where it's going wrong.
• "More within an Assembly":  This is indeed a little bit of a nuisance.  But you can right-click the part and pick "Find in Browser" (or CTRL+B on keyboard) to jump to it without trying to scroll up and down to find it.
• Setting sub-assemblies to a certain texture/color:  You need to learn about View Representations.  I'm not going to write a full explanation of them right now, but they're going to be the solution to your issue.  Right now you are (unknowingly) telling these different levels to remain independent in color instead of matching.
• Copy with mates:  Correct, this doesn't exist.  Some tools in Inventor may provide similar benefits in certain circumstances, but there is no direct equivalent to this feature.
• More on assemblies (editing a sketch dimension):  Why are you complaining about a clear advantage of Inventor?  Inventor maintains the logic that was used to develop the value, in an editable form, instead of just distilling it to a final number.  On this point, Solidworks is clearly inferior based on your explanation, due to the loss of formula history.

[James_Willo · Accepted solution]

Hi Corey, welcome to Inventor! I'm not going to comment on which is better as clearly I am biased, but I have a few answers in addition to John's post above. 

As well as pressing ctrl+B, on more recent versions there is an 'autoscroll' option in the hamburger menu at the top of the model browser that will always show the part on screen when you click it. Also works for features in the part environment. 

There are a few ways to place with mates. iMates and drag and drop two previously mated components from the browser to the graphics area. I get that it's not as convenient as the SWX method. Fasteners has autodrop which is much quicker than the method you describe, but is an all or nothing approach. 

I'm not sure what you mean by 'Inventor drops your part from space.' As far as I know when you place a component, the origin of that components is attached to the mouse cursor until you click. 

Your assessment of appearances is probably running into the issue of appearance overrides. As John says, check view reps, but also there is a clear appearance override button on the top bar.  If using in drawings, make sure you have view rep associative turned on. 

You can tie dimensions to iProperties using the formula    =<parameter name>   The parameter must be set as export in the parameter window also. You're right that the iProperties dialogue is not modeless though. 

Not sure why you can't make a titleblock for A0? I've definitely created A0 drawings before. 

I think you are not using mates correctly. 3 mates should always stop movement of a part. Adding 1 mate should still allow movement, even 2 can sometimes still allow movement. Occasionally they could be other factors stopping the movement, but in general it should work as you expect it to. 

[corey_danielson · Accepted solution]

Thank you for the feedback, sorry for the extensive list, but it's something I have been putting together for the lats 5 months. As I said, I am not badmouthing inventor. I admitted I just may not know how to do certain things.

I am going to delete items on my word document as they are solved. 

• Basic Commands (Zoom Extents):  In Inventor, you don't need a button for "Zoom Extents".  Double-click the middle mouse button.  Did not know this, now I do. Thank you

• Copy with mates:  Correct, this doesn't exist.  Some tools in Inventor may provide similar benefits in certain circumstances, but there is no direct equivalent to this feature.  I will look more into this, see what I can find.
• Setting sub-assemblies to a certain texture/color:  You need to learn about View Representations.  I'm not going to write a full explanation of them right now, but they're going to be the solution to your issue.  Right now, you are (unknowingly) telling these different levels to remain independent in color instead of matching.  I will research this more, sounds like I am just not doing it right.
• More on assemblies (editing a sketch dimension):  Why are you complaining about a clear advantage of Inventor?  Inventor maintains the logic that was used to develop the value, in an editable form, instead of just distilling it to a final number.  On this point, SolidWorks is clearly inferior based on your explanation, due to the loss of formula history. Although I am sure there may be times seeing the logic that was used may be important, I do not remember ever needing that.
• "More within an Assembly":  This is indeed a little bit of a nuisance.  But you can right-click the part and pick "Find in Browser" (or CTRL+B on keyboard) to jump to it without trying to scroll up and down to find it. This answers that question, Thank you. Works perfect (I did now know that)

Thanks for the answers, that is very helpful

[Frederick_Law · Accepted solution]

When you only have a hammer, everything is a nail.

Of course it's difficult to hammer in a screw.

Find and learn how to use a screwdriver and you'll feel better.

Same with any software.  Go through all the "tools" and learn how to use them.

Each software is designed differently.  So forget what you know and start new.

Used SW since 2005.  IV since R1.

BTW I don't like SW.

[kresh.bell · Accepted solution]

> I have used SolidWorks for the last 13 years

I really feel sorry for you, I was also in the same trouble for a little less time

[andrewiv · Accepted solution]

What version of Inventor are you using?  Some of the answers will be different depending on the version.  I have a good deal of experience with Inventor (IV) and some with Solidworks (SWX) so I will add my comments to some of the items.  I can say that there are some things in SWX that I prefer over IV, but I prefer IV over SWX as a whole.  That is probably because I have more experience with IV.

• Pack-N-Go:  As was already suggested, you should look at Design Assistant or if you are also using Vault then Copy Design is a better way to go.  Copy design allows you to copy the top assembly and replace or copy components and drawings and rename files and it sounds like that is what you are after.  Design Assistant will allow similar functionality without vault, it's just a little clunkier to use IMO.
• Constraints:  I'm not sure what the complaint is here.  Everything you are describing about SWX, IV can also do there are just a couple different ways to get there (Constraints, Joints, Assemble).  I think Assemble is closer to what you are referring to with Smart Mates. 
• Constraints:  I would never ground components after constraining them.  I very rarely ground more than one component in an assembly, this is the same no matter what software I'm using.  Usually if something is flipping inadvertently it means that something is wrong with the constraints that are applied.
• Constraints:  If a part cannot move after applying only one constraint then something else it going on.  I have had it happen before where flexibility will cause this to happen.  This can also happen if there are errors in the file.
• Creating custom templates:  As far as I know, everything that you can do in SWX with drawings you can also do in IV.  If you have a specific issue, please post about it and you can get help.  As for the not being able to edit a part from the drawing, there is an application option to allow part modification from the drawing and to retrieve the model dimensions on view placement.
• Regeneration:  When a part changes, you should be able to click the update button in the assembly to see those changes.  If that is not working, then like some of the other issues there is something else wrong.
• Editing parts in assembly:  If you double click on a part in an assembly, it should go into edit mode and you will be editing that part the same as if you opened it up by itself.  If you already have it open then it will switch over to that window and you can edit it.  If you want to see the features in the assembly browser then you can click on Modeling at the top of the browser.  That will show all the features in the parts and hide the assembly relationships.
• Extrusions within an assembly:  You can dimension extrusion profiles from edges of existing parts, but you will need to project the edges that you are trying to use or have the application options set to automatically project them.
• Flexibility:  This can be tricky sometimes in Inventor.  If you can provide more context (screenshots, IV files) then maybe we can see what the issue is.
• Copy with mates:  This is one of the features of SWX that I really do like and wish that IV would develop the same feature.
• More on assemblies:  When I put parts into an assembly the part drops where I click.
• More on assemblies:  This is another one that I do actually like in SWX.  IV always behaves the same as it does in SWX when you add an equals sign before the sketch dimension.  So it will always have the formula and not the result unless you type in the result.

[jtylerbc · Accepted solution]

---

@James_Willo wrote:

As well as pressing ctrl+B, on more recent versions there is an 'autoscroll' option in the hamburger menu at the top of the model browser that will always show the part on screen when you click it. Also works for features in the part environment. 

---

Good catch.  I'm aware this was added, but forgot to mention it since I'm still on a version (2021) old enough to not have it.  This is an option I'll be turning on whenever we finally get around to upgrading, but for now I'm used to getting by without it.

[corey_danielson · Accepted solution]

thank you for your response. I have been trying some of the different suggestion from others, and my list has gotten a little smaller. (I admitted in my initial post that I am fairly new in Inventor, And I was asking people to tell me where I was wrong. I have been getting some great suggestions that I didn't know.) Thank you very much for your answers.

Is there any support (phone) for Inventor? 

[corey_danielson · Accepted solution]

Thank you for your info! It is appreciated. As far as Pack and go.

If I have an assembly, 2 subassemblies within the assembly, along with misc. parts under each subassembly.

Numbered as so:

Top level assembly: BOX

Subassembly 1   BOX-1

Misc parts in Sub Assembly 1   BOX-1-1, BOX-1-2, BOX-1-3

Subassembly 2   BOX-2

Misc part in Sub-Assembly 2   BOX-2-1, BOX-2-2

Misc parts:  1000-262, 1000-393

SOLID WORKS:  Click "pack and Go"  

Select replace

Old Name: enter "BOX"

New Name: enter "CIRCLE"

Deselect items that were not changes.

Select location and hit: Enter.

I have a new assembly "CIRCLE"

Sub-Assemblies "CIRCLE 1 AND CIRCLE 2"

Misc parts "CIRCLE-1-1, 1-2, 1-3

Misc Parts "CIRCLE-2-1, 2-2

Misc Parts 1000-262, 1000-393

This works well with big assemblies; can you explain the steps with inventor to accomplish the same result? I did use this the create standard models at my previous job, significantly reducing the time it took to create a new model, for a similar product.  This particular example would take approx. 30-45 seconds. I am trying to find out how to accomplish the with inventor. Thank you for any info on this.

[corey_danielson · Accepted solution]

I just finished watching a 29:06 long video on Inventor Pack and go. I am assuming this is fairly quick as well.

[jtylerbc · Accepted solution]

I think that was mentioned in this thread already, but it was probably in one of the longer posts and got overlooked.  I think the issue here is that Inventor and Solidworks both have something called Pack and Go, but they don't do exactly the same thing.  What you actually want for renaming Inventor files is Design Assistant.  

In Inventor, Pack and Go is specifically a tool for consolidating files to move to another computer, send to another company, etc.  It doesn't really do anything else, including file renaming.  It sounds like in Solidworks those two functions were built into the same tool.  That honestly sounds like a pretty good idea to me if that's true, but it isn't the way it was done in Inventor.  

[Anonymous · Accepted solution]

@corey_danielson do you have a reseller? Do they offer training?

I'd seriously consider getting whatever training you need/desire. It'll pay for itself 10 fold if not more.

The sooner you get such, the more the payoff down the road. You'll get beyond the basics and learn how to get the same (or better) results in far less steps and aggravation.

[corey_danielson]

Thats it for now, I will post individual questions when they come up. Last question, can I close this post? if so, How?

[joshUTZNH]

The "pack-n-go" functionality you are looking for is in a command called iLogic copy design. It is on the home page tools tab on the ribbon in the iLogic panel. It is not as good as the SW version of pack-n-go but close enough. it may pay to work out a file naming convention that works better with the iLogic copy design method.

I wish inventor had the copy with constraints that solidworks does. that is about the only thing i miss from solidworks though. 

i found solidworks was too forgiving of bad modelling practices meaning it would work, and typically well, until it didn't and then all hell wold break loose. you do need to be more deliberate and disciplined with Inventor and it can take longer to do some tasks, but if done correctly inventor is FAR more stable and reliably repeatable. some of the things you are experiencing sound a little like they are coming from bad modelling practices more than software functionality issues.

for example, using assembly features CAN be extremely problematic and typically should be avoided if possible in both SW and INV. the grounding of a component with one constraint although doable by definition creates an automatic over constraint of the component. grounded is fixed in 6 deg of freedom, the constraint is additional to that. that is where the conflict and issues come from.

i would encourage you to stick at it and look closely into top down modelling using derived parts in inventor as this sounds like it would fix a lot of the issues you are having with constraints and placing parts as well as updating parts. it is also a FAR better way to work generally speaking in both SW and INV. it will also make copying designs and updating the new design with different dimensions super simple. also look into naming your constraints (the important ones) and then using the parameters dialog box (fx button found in a few places) to modify constraints and get the model to update. naming a constraint is as simple as typing the name into the dimension dialog box with an = and then the dimension. e.g. OA_Length=18" or Inside_Depth = 1000mm

for the record, i used Inventor for 4 years full time before going to solidworks for 5 years full time and then 4ish years of using both at the same time before going back to only using Inventor for the last 3 years. i would say that my time with both programs saw me about equally proficient in the use of both including being an administrator and in the implementation of EPDM for a large firm in one of my roles. i refuse to use solidworks again as i find inventor to be that much better in day to day use and with their bug fix, update and development path. i know the change is difficult and keep your positive attitude and approach to it. it will be worth it!