Solidworks to Inventor

[Anonymous]

Yes, I am sure I am not the only one who has transferred from Solidworks to Inventor or vice-versa...

I have 7 years experience running Solidworks and well over 20 years using various Autodesk products (mainly AutoCAD), but have never used Inventor. I am currently taking advantage of the opportunity to use Inventor on an educational basis so that I can teach myself the program and be able to make my resume look better to prospective hiring managers.

From what I have found, the two programs are very very similar. The main differences I have found will be addressed in this email so that I can see if a work around exists I am sure that there have been posts similar to this one - and I promise I searched first but my requested search churned away for 5 minutes and did not produce anything...which was probably my computer's fault or my internet connection. So, I ask that you forgive me if I ask any questions that have been covered numerous times in the past (thank you in advance):

- ALSO, my apologies, up front, for making so many comparisons to Solidworks in this posting. I am just trying to set my Inventor program up so that I am as equally proficient in either program.

1) In Solidworks, when I held down the wheel button and drug my mouse, I would rotate and spin my model. When I held down the shift key and used the wheel button, this would allow me to pan around on screen. As you know, this is completely opposite (and backwards to me) in Inventor. Is there a way to flip these actions so that it would have the same actions that I am used to in Solidworks?

IN other words, I want to rotate and twist my model by pressing the wheel button only...and pan when I use the shift key and the wheel button.

2) When inserting the first part in an assembly (Solidworks), the first part would automatically snap to a point and be a fixed entity - meaning that you could not rotate, spin or move that first component without having to do something else first (like put it in "free" mode). It doesn't seem to do this in Inventor.

When inserting any part into an assembly (Inventor), it seems to have free motion until you lock it in with a constraint of some sort. Even when you have subsequent parts inserted, the first part seems to be free and able to move around. Am i doing something wrong or is there a way to lock the first component in a fixed state so that it can not move freely?

3) I am also having having a problem finding the concentric constraint ("mate" in Solidworks) and "between" (can't remember actual name" - this one would place the mated member directly between two objects/faces. Can someone shed some light on this for me please?

4) AND the last one for this go-round...

In Solidworks (stop rolling your eyes, I gave a disclaimer apologizing for the repeated reference earlier), I had the ability to take a cross section view or my part/assembly at any given time. i could also adjust the location and plane of this cross sectional view...how can I do this in Inventor?

Again, thank you for your patience and I am here to learn....

[SBix26 · Accepted solution]

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@Anonymous wrote:

2) When inserting the first part in an assembly (Solidworks), the first part would automatically snap to a point and be a fixed entity - meaning that you could not rotate, spin or move that first component without having to do something else first (like put it in "free" mode). It doesn't seem to do this in Inventor.

When inserting any part into an assembly (Inventor), it seems to have free motion until you lock it in with a constraint of some sort. Even when you have subsequent parts inserted, the first part seems to be free and able to move around. Am i doing something wrong or is there a way to lock the first component in a fixed state so that it can not move freely?

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For this one, you have two choices:

 a. Application Option to change the default behavior

  b. When placing a component, right click and select Place Grounded at Origin:

Sam B

Inventor Professional 2017 R2
Vault Basic 2017
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[swalton]

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@Anonymous wrote:

3) I am also having having a problem finding the concentric constraint ("mate" in Solidworks) and "between" (can't remember actual name" - this one would place the mated member directly between two objects/faces. Can someone shed some light on this for me please?

4) AND the last one for this go-round...

In Solidworks (stop rolling your eyes, I gave a disclaimer apologizing for the repeated reference earlier), I had the ability to take a cross section view or my part/assembly at any given time. i could also adjust the location and plane of this cross sectional view...how can I do this in Inventor?

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1) I don't think so.  You can map your F4 key to a mouse button to spin the model. I bought a 3dConnexion controller and use it in all the CAD packages.

3) I don't think there is a constraint like you want in Inventor.  You can try the symmetric constraint, but I did not find it to be very stable in Inventor 2014.  It may be better in later releases.  See http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-237E701E-A16B-49D5-95C2-FB6528E41217

4) look under the View tab in the ribbon.  See: http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-6810CA07-80AD-4789-A3B5-192A6069267F  Note that these are part of the Design View Representation.  See: http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-9A49CDC1-4DC7-4462-81D7-E18B8339DE0F

[JDMather · Accepted solution]

1. Get yourself a 3DConnexion device.  I spend half of my day in SolidWorks and half in Inventor and half in Creo and half in Fusion (I have impossibly long days).  Get a Space Navigator and you will wonder how you worked in CAD without one.

2. As noted - either right click and Place Grounded at Origin or change the default behavior in Tools>Application Options.  This should be the default behavior in my opinion.

3. Symmetry Mate (what version of Inventor are you using?). Also check out Insert constraint (for cylindrical faces (circular edges)).

4. Not sure why you would be having an issue with this in Inventor.  What version of Inventor are you using?

[Anonymous]

1) I will look in to this device. Not familiar with it, but I am an old school CAD guy who recently earned his engineering degree....(patting myself on the back)

2) I agree..should be default action in my opinion.

3) Will look at symmetry mate to see if this gives me what I am looking for

4) Not having a problem getting it to work - having a problem finding out what I was supposed to do in Inventor vs. SWX...in SWX, it is as simple as clicking on a small on-screen icon (always present)

In general, I am using Inventor Professional 2017. I downloaded the education version (which is a full version from what I can tell) because I am still listed as a student taking some extra classes for engineering (test prep classes). I decided to give Inventor a try because I am already using ACAD 2017 and Advance Steel 2017. We had some projects that were going to require solid modeling in the near future and I thought it would be best to just keeep it all in the same family....so, I decided that in my spare time, I would teach myself Inventor and when the time comes, we will purchase whichever software I dictate.

[Anonymous]

I accepted the two solutions as they seemed to be the most related to what I was looking for. Personally, i would like to thank all that contributed to the discussion.

I am sure I will have many more questions - right now, I am just having fun with the program and trying to learn it.

Please keep any additional suggestions coming

[rdyson]

4) AND the last one for this go-round...
In Solidworks (stop rolling your eyes, I gave a disclaimer apologizing for the repeated reference earlier), I had the ability to take a cross section view or my part/assembly at any given time. i could also adjust the location and plane of this cross sectional view...how can I do this in Inventor?

I have a button assigned on my Space Pilot for this. IF you haven't already found it, check out F7 while in sketch mode.

[Anonymous]

Tried using the F7 key...seems to make everything, except for the active sketch, disappear. Is that what it is supposed to do? Not 100% what I was looking for, but could come in handy and I appreciate you sharing that with me.

I do a lot of integrated machine design. I like using the section command (SWX) because I could get a real look at what I was doing and could see the clearances first hand - without having to go through the process of changing transparency on some of the items.

So, I have found a few other items that I need to know how to do, or where they are...

In assembly mode - is there a Parallel Constraint? I will sometimes use planar faces to mate as parallel just to get the parts in the correct orientation for the assembly.

In sketch mode - is there not a mid-point constraint?

In sketch mode, is it possible to turn off the vertical and horizontal lines that are visible after you select the plane to work off of? In SWX, after choosing the plane, all of the lines would go away. You would have faint visible lines show up when you had your cursor in the vertical or horizontal positions that coincided with the center of the vertex (UCS point) and I believe you may have had a point at the UCS center or maybe it was just a very small UCS - trying to go by memory and I haven't worked in SWX in about 2 months - all of this just comes second nature when you are working within the program and I forget what some things are called...I just know where they are and what they do.

And for those that suggested, i did go back and look at the 3DConnexion device...I have got to try and figure out how that would work with my system and how i can convince the boss to purchase. Any one know if this is compatible with Advance Steel - which is my main program?

[JDMather]

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Big_Deddie wrote:

In sketch mode, is it possible to turn off the vertical and horizontal lines that are visible after you select the plane to work off of? ...?

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Tools>Application Options>Sketch tab - turn off the Axis visibility (should not be needed).

http://forums.autodesk.com/t5/inventor-forum/skillsusa-document-now-on-screencast/m-p/5856691/highli...

[rdyson]

F7 takes away everything in the foreground so you can see the sketch without switching to wireframe. "Foreground" depends on you view direction.

Use angle constraint to lock planes parallel.

Not sure how you would use midpoint in SWX.

I'm not aware of a way to turn off the axis lines and would not want to if I could. You need them to know which is vertical and which is horizontal since the sketch isn't necessarily orientated to the screen.

I have no knowledge of Advance Steel but I would be surprised if the 3D controllers do not work with it. They work with a wide variety of apps.

[JDMather]

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@rdyson wrote:
...Not sure how you would use midpoint in SWX.

I'm not aware of a way to turn off the axis lines and would not want to if I could. ....

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I use Midpoint all of the time in both Inventor and SolidWorks.  Midpoint is simply a Coincident constraint (relation).

I never have my axis lines visible.

[rdyson]

Not knowing SWX, I assumed from the OP's question that there is a separate midpoint constraint plus a coincident constraint.

Also assumed that the OP was referring to the below axis. How can they be turned off?

[JDMather]

In SolidWorks there is a separate Midpoint constraint and Coincident constraint.

Inventor uses Coincident for both.

The axis can be turned off in Tools>Application Options>Sketch tab.

[jholland3XDLM]

First of all thanks for taking the time to use Inventor before talking about how Solidworks works differently. Looks like your first two points have been well addressed but I will include them as a recap. As with any CAD program there are many ways to customize and model parts the following is simply my solutions to these similar problems:

1. Pan, tilt, zoom, rotate.   No good way, get a 3D mouse, it is your friend. 

                                   or   try "steering wheel" or "view cube" controls. You may have to learn new shortcuts to use effectively.

2. Ground first part at origin.  Change "Application options" "Assembly" tab  "Place and ground..." 

                                    or        right click before placing first part (this also works if you want to rotate a part before placing it).

3. Mid plane , between or whatever SW called it. (I forgot the name as well)

                                            Use constraints to mid-planes. May have to change modeling practices to create parts with origin planes bisecting your part, or add these planes where you want them to be later.

                                or          Combine other constraints. Insert does this for you for cylindrical objects such as a bolt into a bolt hole. Not sure about this but it seems to move your first selection to your second selection adding constrains that basically make your selections both concentric and coincident. The regular "mate" constraint works with multiple surfaces, if selecting two cylinders, it becomes concentric while not locking in any coincident constraints. It also works for "between (SW)" when selecting planes. (IE. make two planes coincident)

                              or            use sketches to constrain, this method is best for some applications while worse for most.

4. cross section view     This is located on the view tab / appearance. With options for "quarter section view" "half section" " three quarter" and "End section" You can right click on your toolbar (anywhere) to edit "user commands" to add this button to your main toolbar, or drag it down to have it on a floating toolbar.  If using either "quarter" views, Inventor will ask for two planes (or faces) to represent where the section view originates and a value for how far the cut is. The "Half" command only asks for one set.  You can also click/drag for a rough guess section view. "End" simply ends the section view and returns to a normal view.