Assembly Constraints - Autodesk Inventor Assembly Tutorial | Autodesk Inventor 2021 IN DEPTH

[Calm Hip-Hop Music] Hey everybody it's Alex with Engineering Applied in  this video I’ll be giving you a detailed overview   of the assembly constraints found within an  Autodesk Inventor assembly file if you want   more easy to understand and practical content like  this made by an experienced engineer like myself   make sure you like this video subscribe to the  channel and turn on notifications so you don't   miss out on any helpful content like this in the  future if you're looking for a specific function   check the description for time stamps and if you  don't find what you're looking for in this video   make sure you check out the other videos in my  Autodesk Inventor series playlist because I know   you'll find exactly what you need there let's  get started okay everybody so here we are in   our assembly file and for this practical example  we'll be taking a look at a draft shield that I   modeled up so essentially what a draft shield does  is we put a high precision scale on the inside of   this enclosure and the shield will prevent any  of the air from our HVAC system from blowing   on the scale directly and ruining the stability  of our measurements additionally this enclosure   keeps out any sort of foreign objects or debris  from getting on the scale itself and potentially   ruining an extremely expensive and precise piece  of equipment now I’ve used these enclosures quite   a bit in the pharmaceutical industry and I wanted  to share my experience with you because I always   like to connect the dots between these lessons  and reality so that you get more out of them   so the way this lesson will be structured is we'll  take various design elements from this assembly   and apply the relevant constraints to those design  elements so that we can get our desired result   without having to build this thing from the ground  up and wasting a bunch of your time so the first   constraint that we want to take a look at is our  mate constraint so here I have just some frame   pulled up so this is t slot frame in our 3D  space and this is the beginning of our enclosure   assembly itself so if we go back to our enclosure  you'll see we're starting with this bottom frame   section here and using the mate constraint as part  of that section okay so we'll go back to this tab   and then now let's go up to the relationship  section and click on constrain after clicking   constrain we get the place constraint dialog box  that pops up and then you'll notice our assembly   constraints tab is pre-selected so in this  video we'll be only looking at the assembly tab   in other videos I cover the motion constraints the  transitional constraints and the constraint set tab   individually just to make it easier for you to  navigate moving back to our assembly tab and   going down to our type section here this is where  we can select the type of assembly constraint that   we want so you'll see we can pick up our mate  constraint that's this first one here and let's   go ahead and start making some constraints so  let's move over to our selection section where   we can pick up the various geometrical elements  we want to use to create those constraints with I   went ahead and scrambled up the parts in 3D space  a little bit so that we can get them back into   alignment using the mate constraint so what we  want to do first and I generally recommend doing   this when you create a new assembly is find the  first part that you want to ground at the origin   or position in 3D space such that you can build  off of that one part that way the whole assembly   doesn't move around and you have a strong anchor  point as you go through and build your assembly up   so when we anchor the first part what I’m going to  do here is I’m going to snap the origins the local   origins for this t-slot segment here with the  global origin that's associated with the assembly   itself so let's go ahead and snap this yz plane  to the yz plane of the assembly okay we'll hit   apply and then now let's go ahead and select  the xz plane with the xz plane of the origin   okay hit apply and then now let's snap  the two center points to one another   okay hit okay and then now when we go to click  and drag the part it's not going anywhere and   now we have a stable anchor point for the rest of  our assembly Alternatively you can use the place   command to bring in the part that you're going to  use as your anchor point and before you drop it   you can right click and then select place grounded  at origin okay so it'll drop it into 3D space   and now when we click ok and go to drag this  around it's not moving because it's currently   grounded and you know it's grounded when you see  that little push pin with the ground symbol next   to it now before we move on I want to go ahead  and address a major detail here when using the   selection filter and that is which part moves to  which part well whichever part that you select   first will move to the part that you select second  so for example if I want to mate this front face   of this part to this front face here I would  select this one first because I want this part   to move so the part you want to move you select it  first and then let's select this one here second   so we'll select that face there and you'll see  they snap together now that they're connected   face to face I want to go ahead and make another  point here and that is the solution section so   the solution section governs what the output looks  like so the first option is mate and mate will put   those faces I’ve selected facing one another  this way if I select flush it'll take those   original arrows that are normal to the faces that  I selected and align them in the same direction so   if I select this it'll flip it in the other  direction and it'll make it flush with one another   taking a step back let's take a look at this  option here which allows us to pick the part first   and then the specific geometrical element we want  to use to create that mate with so let's go ahead   and check this box and see what it does so when  I check this box and I hover over my part of   interest you'll see the entire part is highlighted  first so without this enabled I pick up the   individual geometrical element okay but let's  say I have a complicated assembly where there's   a section that I want to pick up but it's housed  within the assembly itself and I can't really see   that section to pick it up well what you can do  is you check this box and then you hover over the   piece that you want so let's say I wanted to pick  up an element that's behind this piece and I can't   see it so I can hover over this rail left click it  and now I can pick up the geometrical element of   interest and when I hover over this part it  doesn't give me any selections so that is some   extra control that I have available to me by  using the pick part first option so now I can   pick up the element I want so let's go ahead and  just snap this face to the front of this again   pick this rail okay and then we'll select this  front face and then it'll snap those two facing   one another and then I can hit okay moving down we  have our offset section so this essentially does   exactly what it says and we can create an offset  using this value so let's go ahead and create   an offset between this top face and the bottom  face of this rail so we'll select this top face   because this is the part we want to move first and  let's move it up to this bottom face okay and once   they snap together we can go into this offset box  and type in a value so let's type in half an inch   okay so now that we typed in 0.5 it creates a  half inch offset there and if I were to hit ok   you'll see that I can move these parts around but  it'll always maintain that half an inch offset   additionally what you can do is after snapping  these two parts together so I’ll just repeat   that operation you can actually measure a feature  dimension within your model and use that value as   your offset value so click this right arrow here  and go to measure and let's say for example I want   that offset to be equal to the thickness of one of  these rails or the height of one of these rails so   I’ll pick this bottom face here and I’ll pick this  top face here after I’ve already clicked measure   and it'll set that gap to the thickness or  the height of one of these rails moving down   we can actually toggle our preview option here by  unchecking that box and checking it back on if we   want it so for example let's see what it does when  we have it enabled so we'll just select this face   and this face and you'll see it gives us that  preview but now let's take a step back so we'll   hit cancel we'll go to constrain but let's uncheck  this first now let's go ahead and pick up our same   two faces and when we do that the part doesn't  automatically snap in place and give us a preview   but when we hit ok it'll fulfill that command  for us so just depending on your preference   within your workflow you can either enable  or disable those previews this next option   allows the software to predict the offset and  orientation of our two mated parts so let's go   ahead and enable that and let's say for example  that I just was sort of eyeballing the location   of this t-slot frame here and I want to maintain  the gap that I currently have set between this   top face and this bottom face so what I can  do is sort of drag it into place into 3D space   and then now I can go ahead and click  this top face click this bottom face   and when I do that with this option checked it  will automatically set that offset value in my   offset box okay so um this is really helpful  for when you just want to eyeball the location   and offset of various components within your  assembly and you don't exactly know what that   offset is going to be so you can enable this it  will retain that orientation or try to predict   that orientation and offset for you moving down  we have our name field and this is where we can   enter a custom name for our constraint so let's go  ahead and click in this box and let's just type in   example okay and let's go ahead and set this  surface flush with this top surface here on this   rail now you'll notice it gave me the incorrect  solution it gave me mate so I want to go ahead   and switch this to flush so it sets those two  arrows in the same direction rather than opposing   directions okay so now that we have that we'll hit  ok and underneath the t slotted frame number three   you'll see that the relationship that's applicable  to that frame it says example so that's that mate   that I just applied with that custom name let's go  ahead and continue on down to our limits section   and if I didn't mention it before the way you  access this extended menu is you click on these   little arrows in the bottom right hand corner of  your screen for the additional menu options so   essentially what the limits allow us to do is  it allows us to set a range for the movement   of the mate between our two components let's  go ahead and mate this face to this face here   okay we'll go ahead and set an offset value  of half an inch and this first checkbox   essentially allows us to set whatever is in our  offset box as our resting position so that is   this gap in our assembly by default okay so by  default we're going to keep that half inch gap   and then we can enable or disable our max and min  values for the distance between these two faces   so let me go ahead and rotate this around okay  and let's set our maximum value to two and a   half inches and we'll set our min to 0.250 okay  so our minimum separation will never fall below   a quarter of an inch and then our maximum  will never go above two and a half inches   so once we have those parameters set we can hit  ok and I want to note that I am going to ground   this in 3D space so that this can't move around  so I’m clicking and dragging this it's not moving   so I’m going to click and drag this part I  can bring it in but you'll see it stops as   I’m pulling it over you'll see that mouse cursor  moving to the left the part won't actually go   below a quarter of an inch and gap between the  other rail now let's go the other direction so   I’m pulling it outwards you'll see it stops at  two and a half inches okay now one thing I want   you to notice is when I let go of left click on  the mouse it pops back into its default position   so it works in both directions so we've seen that  we can mate faces to one another edges and so on   and so forth but what about rounded or cylindrical  features well in this particular case what we can   do is we can mate this open side of the hinge to  this pin on the fixed side of the hinge okay so I   have my door its free floating in 3D space so what I  want to do is go to constrain okay make sure it's   on mate and then when I hover over any rounded  feature so I’ll hover over this outside piece   you'll see that dashed line that's the axis that  runs through the center but in this case we want   to pick up this pin here so we'll left-click and  you'll see it selects the axis and you'll see the   axis direction green arrow is pointing up okay so  take note of that so let's pick this intersection   and it snaps the two together now over here in  the solution section this is where we control   the alignment of our two constrained parts  so currently it's on opposed so the arrow for   this segment of the hinge that's attached to the  door panel is facing down and this arrow on the   stationary portion of the hinge is facing up so  they're going in opposite directions this is the   opposed solution we can also align it so when we  click that it actually inverts the door and puts   it inside out okay so now the two green arrows  are facing in the same direction we actually   don't want it that way now the last option is the  undirected solution option so essentially all this   does is instead of defaulting the orientation to  opposed or aligned it just snaps it to its closest   axis so for example we can actually set undirected  by default and then when we're working with our   model we can manually move and rotate the part  around get it close enough to the final position   and then use undirected to finally snap it  into place rather than risking it inverting   into a different orientation if we don't want  it to do that and of course everywhere else   in this dialog box for this particular type of  mate constraint we have the same settings so   we have offset we have the prediction setting  we have our limits and so on and so forth now   let's go ahead and complete this constraint so you  see we've snapped the two axis elements together   but the gap between these two hinge elements are  sort of off a little bit okay so let's go ahead   and apply the first change but then let's go ahead  and set a mate constraint between this top face   and the bottom face of this stationary hinge  element okay let's set this offset to about six   thousandths of an inch that should be close  enough to what we need it to be we'll hit   okay let's go to this view here so we can get a  better look at it our gap looks pretty even there   and uh now let's see what happens when we click  and drag on the handle now you can see our mate   constraint is exactly as we intended it to be  the next constraint we want to go ahead and take   a look at is the angle constraint so using the  angle constraint we're going to set the angle and   travel of this door so you can see currently  it's able to free spin all the way around we   don't actually want it to be like that so what  we're going to do first is we're going to go to   constrain and then click on angle and you'll see  here in our solution section we have three main   solutions our first solution is going to be the  directed angle solution so what we want to do   is pick our first element on our moving component  which is going to be the door so let's select this   front face here and you'll see that little green  arrow is normal to that front face so that's our   selection in this particular case and then let's  go ahead and do the same thing on this cross bar   okay and then let's go ahead and set an angle  value now one thing I want you to note is in this   particular case the angle is set counterclockwise  again we're using the right hand rule and so if I   want the door open out here somewhere in space at  135 degrees from this direction I can either type   in 225 here and it'll open up the amount that I  want or I can type in negative 135 and it'll go in   the opposite direction but it'll achieve the same  result now let's go ahead and click ok and see   what happens now you'll see that I clicked ok but  when I click and drag this that angle is set in   stone it's not going to move anywhere and that's  not necessarily what we want in this case because   we want to control its opening and closing  abilities based on that angle so let's go   back into the angle constraint and take another  look at this so let me delete that first go back   into constrain click angle and then let's take  a look at our second option our undirected angle   so following the same order of operations as with  our directed angle let's see what happens with   the undirected angle so we'll select our front  face on the door our front face on the crossbar   let it snap into place and so by default it's  ending up at zero degrees with the door closed   so now one thing I want you to notice is if we  scroll down to this additional extension of our   menu we have the ability to set limits since we  want the door in its closed position to be our   resting position let's go ahead and check this  box here that says use angle as resting position   we have zero in that box okay so now we need to  set our maximum and our minimum values for our   limits so our maximum is going to be 135 degrees  and our minimum is going to stay at zero now I   want you to notice the behavior of this when we  use the undirected angle option I’ll click ok and   then let's go ahead and grab this handle and pull  it open and see what happens okay so I’m pulling   it open and it gets to a certain point and it just  sort of freezes there so let me try that again   so I pull it out and it sort of stops okay  it locks into place and then when I let it go   it snaps to the other side well that's not exactly  what we want and what's happening is past its   zero point it's able to rotate 135 degrees in  either direction so that is what the undirected   angle allows you to do so if you have an open  door to where it's able to swing on either side   this would be the ideal option for you but in this  particular case this is not what we want since   we need the door to stop at the zero position now  notice because I set the resting position at zero   degrees when I pull it off of zero degrees and  leave it sort of in that area and then let the   mouse go it clicks back into position so on either  side it rests back at zero but again that's not   exactly what we want so let's move on to  the next option and see if we can achieve   what we're looking for so our final solution  option is the explicit reference vector option   here we can select the cross product vector or  the z axis for this operation which will limit the   rotation direction to a single direction let's go  ahead and click our first entry which will be the   front face of this door we're repeating our steps  just as we did before and then we're going to   click this front face on the crossbar and then we  have a third selection for our reference vector so   let's go ahead and click one of these edges here  to use as our cross product vector and then now we   go to our angle box we want to leave it at zero  because we want zero degrees to be our resting   position but if you're unsure which direction this  is going to rotate you can go ahead and enter a   value so we want to be at 135 degrees and you'll  see it rotates out to the proper area you could   set negative values to see what happens when you  do that so it'll go in the opposite direction so   depending on what you want you can type in those  values accordingly so let's set that back to zero   okay and let's use that as our resting position  toggle our maximum value on and set that to 135   degrees so that way the door can only go out to  135 degrees and then we'll set our minimum to   zero degrees let's hit okay and there we go now  let's go ahead and test out this door handle so   let's go ahead and click and drag our handle so  I’ll go ahead and rotate this around a little bit   clicking and dragging and once I get past a  certain point you'll see that the door snaps   back to zero so I’m hitting my 135 degree limit  and then it snaps back to zero let's go ahead   and try to go in the other direction so I’m going  inwards and you'll see it doesn't move past zero   degrees that's exactly what we want to do in this  particular case since we have this little magnetic   latch here that doesn't allow it to go beyond zero  degrees now let's say for example you want to go   in the other direction so what you want to do is  making the same selections we'll select the door   cross bar and then our reference vector we want  to go inwards by 80 degrees so let's go ahead and   type in negative 80 degrees just to verify that's  the direction we want to go and that looks correct   so what we want to do in this case is set this  back to zero if we want the latch area to be   our zero position what we can do is use that as  our resting position toggle max and min on but   this time our maximum is going to be zero degrees  and our minimum is going to be our limit in this   direction okay so we can type in negative 80 there  now um let's try to type in negative 80 here and   put zero here you'll notice the number is put in  red because it's out of range the software doesn't   understand what we're trying to do here because  of our cross product vector so we just need to   invert these two values so again this will be zero  and since we're going the negative direction we'll   use our minimum value to set that limit in this  direction negative 80 hit okay and then now this   time I can't pull the door outwards but I can push  it inwards and it'll stop at 80 and then it'll   snap back to zero our next constraint type is the  tangent constraint so with the tangent constraint   selected in the type section what we're going  to do in this example is constrain this curved   surface on this caster wheel to this flat surface  on this plate here so what we want to do is select   the curved surface on our moving part then we want  to select the flat plate that it's constrained to   when we do that you'll see it snaps into place  and we have two solutions that are available to   us so currently it's set to outside so that means  the wheel is outside of this plate sitting on the   surface if we select inside the wheel will go to  the inside of that surface so depending on what   you're trying to do you have those two options  available to you and of course you can set your   offset value name your component and set your  limits as necessary so let's go back to outside   we'll click ok and then now when we move this  part around it rides on that surface okay so   it's tangent to that surface at all times our  next constraint option is the insert constraint   so what insert allows us to do is it allows us to  align multiple axis elements and snap edges to one   another so in this example what we want to do here  is we want to thread these fasteners through these   holes and then secure them with these cap nuts  on the other side just like you see up here now   the distinction between the insert option and the  mate option is when we select mate it only picks   up the axis in the center but the problem here  is when we you know connect that to this axis   and hit ok I can still move this fastener in and  out of this hole now what will happen when we use   the insert option is it'll do two operations  with one step so let's go back to constrain   we'll go back to insert okay now let's pick up the  same area but you'll notice I see an edge with an   axis so let's pick up this edge and axis by  clicking once it'll select them both at one time   and then let's select the edge that that bottom  uh surface of the screw will rest on so it's going   to be this edge here we'll select that it snaps  into place we can also change the solution here   so currently it's opposed we can align it as well  but we want it opposed let's go ahead and click ok   now this time when we click and drag the fastener  it doesn't move in and out it only can rotate but   we can actually fix that as well so if we go back  into here we can go ahead and lock the rotation   so let's take a couple steps back okay let's try  that again go to constrain insert we'll select   the fastener okay we're going to select this edge  because this is where we want it to rest against   we'll go ahead and pre-select this lock rotation  option okay we'll go down to our spot that we   want to rest it on which is that edge there you'll  see that our rotation is locked and when we hit ok   now everything is completely locked down it  won't move in and out and it won't rotate   so if you're trying to place a bunch of fasteners  quickly this is a good way to do it now let's go   ahead and do the same thing for the cap nut on  the other side so we'll go to constrain insert   okay let's rotate this around a little bit zoom in  on this part we'll pick up this edge here okay and   then let's go down uh to this fastener on the  other side we'll pick up this edge here in the   door panel and you'll see it locks into place and  then we can lock the rotation once again and then   of course you have your offset options your limit  options your naming options we'll hit ok and there   we go now everything is locked into place and when  I click and drag on that cap nut it's not moving   anywhere and then we can repeat those operations  for the second set of fasteners down here put them   into place and then move along as intended our  final constraint type is the symmetry constraint   so with the symmetry constraint we can keep these  t-slot frame segments symmetrical about this   yz plane so we'll go ahead and make our first  selection so I want this first face and the second   face to hold symmetry about this plane okay now  um you'll notice we have a third selection filter   this is to select our symmetry plane which is this  yz plane okay and then now we can set our solution   type so currently these green arrows are facing  one another that means they are opposed okay   we can also align them so you'll see this part  actually flips around so the entire part flips   okay um so that will give you an aligned  solution um so let's go ahead and go back   to opposed and then of course you can rename  this entity as well we'll go ahead and hit ok   and now when I click and drag these components  they move with symmetry about that yz plane now   before I go ahead and wrap up this video there's  one last thing I’d like to discuss and that's   using the ALT key on the keyboard to create mates  without actually going into the constrain option   up here in the relationship section so in this  example all we're doing is we're going to mate   this front face with this front face and align  two sides to these two sides here so what I’m   doing now is I’m holding left ALT on the keyboard  and while holding ALT you hover over the face of   interest that you want to click and drag and we'll  left click and hold on the mouse and you'll notice   when we pull the mouse away a little bit you  get this blue highlight on the face of interest   and that's the face we actually want to create a  mate with so now we'll move it over to this face   while holding left click and then release left  click and you'll see once we do that we can click   and drag this around and it's mated to that  front face so these two faces are mated but   we want to go ahead and take this a couple steps  further and we want to align this top surface with   this surface and this side surface with this side  surface now let's go ahead and repeat our previous   steps so this time I actually want to grab this  curved edge here and mate it to this edge here so   that we can lock it into place in one move so I’m  holding ALT on the keyboard and then I’m going to   hover over this edge left click and hold I’m going  to drag away just a little bit and you'll see that   edge is selected now I can hover over this edge  release left click it drops it into place and now   when I click and drag this it all moves together  and I didn't even have to go into the constrain   option and use these tools in here to do that  just holding ALT on the keyboard and moving and   clicking and dragging the parts will get this  done for you that's all for this segment of the   Autodesk Inventor Assembly Creation Module where  I gave you an overview of the assembly constraints   I really hope that you found this tutorial to  be helpful and that you put what you've learned   into practice so you can continue developing your  skills as you work your way through these lessons   also before you watch the next video in the series  make sure you subscribe to my channel and turn on   notifications to stay up to date on future content  that will help you create the future you want for   yourself and of course don't hesitate to leave  a comment or reach out via my website contact   page and let me know if there's anything else  you'd like to learn about or see on this channel   I really appreciate you choosing to stop by  and learn with me and I’ll see you again soon [Calm Hip-Hop Music]

Channel: Engineering Applied

Views: 5,019

Keywords: autodesk inventor 2021 tutorial, autodesk inventor tutorial for beginners, inventor tutorial 2021, inventor professional 2021 tutorial, inventor 2021, autodesk inventor 2021, inventor 2021 tutorial, autodesk inventor, autodesk inventor tutorial, inventor, autocad 2021, how to constrain in autodesk inventor 2021, assembly constraints autodesk inventor 2021, assembly constraint command autodesk inventor 2021, how to use constraint in autodesk inventor 2021, assembly constraints

Id: 3H0giE13fZc

Length: 28min 2sec (1682 seconds)

Published: Thu Dec 03 2020