Poor Constraints and Parametric system

[Anonymous]

As per the title the constraints/parametric aspect of this product has been performing awfully. I've been having a mass of issues which I don't have the time to write out fully now but I will attempt to describe some of the issues as best I can below.

I began with a basic square with equally chopped corners (thus an octogon with 2 sets of 4 equal length sides). After managing to lock in the shape (not an easy task by any stretch of the imagination! Note: in the attached file I simply locked the segments in place, nothing at all like what I need in reality it just helps to avoid apparent (false) constraint conflicts when offsetting) I attempted a basic offset with the intention of spacing this out exactly 10mm equilaterally... Except that every single line segment loses all sense of association with the line from which it was just offset. The only relationship maintained in any sense of the word is the links between each segment. So instead of a basic 1 step operation in the fashion of Inventor the following 17 tasks are required:

1. Offset (distance or not, makes absolutely no difference anyway apart from the initial positioning of the offset pieces) the octagon.
2. Constrain all 8 segments parallel to their parent segment (individually)
3. Apply an aligned parametric dimension of 10mm to each segment (individually)

On top of the massive task list to contend with the shape has a habit of unintelligently deforming itself if not carefully arranged prior to attempting the addition of any constraints. This results in many false starts and undo/redo actions.

So having managed this first step then comes the next issue. I don't just need the octagon, I need rounded edges, the center of each arc lying on the parent corner. Applying a fillet with radius 10 to every corner as needed does this... except there is no constraints in place and absolutely no link between the corner and the center of the radius. dragging any of the outer ring distorts everything completely. AutoCAD apparently lacks the ability to constrain the centerpoint of a fillet to anything? I've googled quite extensively and spent the day trying but to no avail. This unfortunately means I am left manually hacking at it to get the centerpoint to stay where its needed. The best solution I found was to set a fillet to the same offset (10mm) and set all fillets to be equal to that fillet.

Now that has one very basic octagon with an offset and rounded ring around it, one very small fraction of a task and yet it took several minutes off roundabout messing to gain any sort of progress. Its also a rather useless ring for several reasons, not least of which if I cut the ring in any location it removes all those carefully crafted associations and we end up with the crumpled bag result very shortly. I don't pretend to have offered up an even remotely elegant solution, it frankly sucks but its about the only one I could find that didn't immediately self destruct itself part way through the process.

It frustrates me no end that such a basic task requires such a tedious solution. Surely I am missing some rather important factors? Does AutoCAD really lack the ability to snap to the centerpoint of a fillet for example (yet I am able to snap to the center of a circle/arc/diy fillet with an arc, 2 coincident and 2 tangential constraints)? Is there some option somewhere to make the necessary associations with the original segments when it comes to offsets? Why is it that explicitly giving it the command to offset by 10mm it doesn't also insert the dimension ensuring it remains thus?

There is also some serious issues going on with the system detecting constraint conflicts in the complete absence of any such situation. Take for instance the following situations:

• Placing a single line (with absolutely no associated constraints) into the sketch and attempting to apply the collinear constraint to another straight line segment (after you get about an hour into a drawing it locks up and you simply cannot apply this operation to any 2 segments in the entire sketch, not even 2 brand new lines placed expressly for the purposes of testing).
• 3 parallel but otherwise freefloating lines (with verified parallel constraints in place to each other and no other constraints attached) and attempt to place the symmetric constraint upon them
• Attempting to constrain parallel an entirely new and unconstrained line to another straight line segment (refer attached example).

All of these situations (and many more) result in the exact same error dialogue in the command bar: "Dimensional value or resultant geometry is inconsistent with existing configuration" and no constraint is applied.

Is this a common error and can it be easily resolved? Why is it that when an error occurs AutoCAD has a fit and doesn't let you do anything instead of offering help (Think the dialogue from Inventor that allows you to click through each and every conflicting constraint). Is there a "sketch doctor" or even just a basic conflict analysis tool in AutoCAD? Is there even just a table database of constraints that would allow one to easily scroll through and view all potential conflicts (given that half the constraints don't show up even when show all is toggled)?

Having worked with inventor quite a bit I am more than familiar with parametric modeling, I know what a constraint conflict is and I know when there is no such issue. Each of the 3 demo points listed above appears to defy the basic principles of the constraint logic. A brand new and unbound line should in nearly every circumstance be able to be constrained with basically any of the available constraints and yet in each of these instances not one option is made available.

I've attached examples where possible/convenient. Unfortunately I am not able to share the contents of some files and others I deleted whole segments/files and redid them when frustration got the better of me. I hope some advice is available, I've just about had enough of this madness and I'm ready to throw in the towel. Inventor just works until it doesn't (thats another story), its a logical, efficient interface, so similar in initial appearance yet worlds ahead of AutoCAD.

Really (Really!) appreciate any assistance that can be rendered,

Branyon

[leeminardi]

I could not follow all the problems you mention  but will agree that AutoCAD's parametric constraints does have it idiosyncrasies.

I think your goal was to create an octagon and then another octagon outside of it but with rounded corners.  Additionally you would like to be able to use parametric features to modify dimensions of the geometry and have the shapes automatically update. Something that looks like this.

There is more than one approach for any geometric construction.  Here's one the worked for me and yields the results I think you want.

Create one eight of the design and use AutoCAD's polar array feature to finish the shape.  The first decision in this approach is to decide which eighth of the shape to create.  I decided I rather have a full arc and the straight sides as two pieces.  Here's the parametric result.

Note that the red construction lines are part of the constraints but on a different layer.  The angles are 22.5°. The red lines have collinear constraints.  You can edit the 10  dim and the radial 7.76. dim and the shape updates appropriately.  The next step is to use   arraypolar   with the ASsociative option set to No and the Items set to 8.  This results in the following where the original linear dim (10) and and fillet radius value can be edited.

I did try using an associative polar array but it was too difficult to edit the shape.

[beyoungjr]

Great job taking a stab at this @leeminardi!  I played with it for a while earlier but I found myself lost in trying to address too many of the concerns that were originally posted (walked away for a while).

Your focus on the initial geometry should help @Anonymous re-think his approach to generating the profile.

I was concerned over his remark about the overall shape being difficult to conceive.  I think he was just taking a difficult approach to the initial construction and when he started trying to constrain, he was mentally tied to his difficulties in his construction process.

The parametric constraints within AutoCAD were surely adopted as a transitional feature toward Inventor, just as the ViewBase functions are.  I think it would be unwarranted to expect all the power and grace of Inventor within AutoCAD.  That said, I think your approach might be a really good process toward applying the parametric constraints on top of the minimal, thus efficient, profile entities.

I encourage Branyon to continue his interaction here at the AKN forums when he wishes to share a problem, a technique, or just participate.  Just need to remove the duct-tape from around my scull after trying to think through too many of those things in the OP;)

Kudos to you on this "trying-to-dry-up-day" in Northern Maryland;)

Blaine

[leeminardi]

@beyoungjr thank you for the kind words.   I've used many different parametric modelers from Designview by Premise in the 1980's (created by Jon Hirschtick) and later PTC's ProEngineer (which became  Creo) to Solidworks and OnShape (both also Hirschtick companies) to Inventor.  Of all of them I find Inventor the most helpful in resolving constraint conflicts. 

In resolving @Anonymous 's challenge there were a few traps.  He was working with a single polyline which did not allow him to reference individual line and arc segments.  It is true that you cannot constrain the center of an arc directly with AutoCAD's parametrics but the tangent constraint enabled the same result. I wish there were a way to easily reference  the intersection of two lines as a constraint.  Instead, I used two lines segments that shared a coincident point and  a collinear constraint.

I used an associative polar array in my first iteration.  Although I got the desired result I found it next to impossible to isolate the original parametric instance to edit and the update the rest of the array.  Opting for the non-associativity may be a little less elegant but enables easy editing. 

It's a damp day here in Massachusetts as well.  A good day to do some CAD!   

[Anonymous]

Hi Leeminardi,

Yes unfortunately I was at the end of my day looking back over the frustration trying my best to explain and model the situations I had been in. As always seems to be the case the issues don't show up when you want them too but I gave it a crack anyway.

Regarding your solution (much appreciated btw, thank you) I do have a few questions which is largely what prevented me going this route. I had used the array approach almost exactly as you did it with one exception: the associative option set to yes. I was under the impression (not that I had googled I'll be honest, but extrapolating from the name itself) that ticking the associated box would mean all elements of the array were associated and by extension should all update as the master was updated? It seemed to work somewhat like I thought it would but simply adjusting the values would trigger all sorts of errors and I ran into the latter issues described in my post which basically rendered that entire file useless, a corrupt of sorts.

I downloaded your file there and opened it up and I note that you ran into the next issue I faced with that particular solution. By attempting to manipulate any given line segment the shape falls to pieces (or when using the center guide line of each segment tears the individual component apart). This applies also to any constraints acting upon the segment at a later date (this basic shape is simply the first stage). I attached your file immediately after dragging on 2 line segments where you can see both the freedom to move and the freedom to warp come into play.

For the array to work in my situation I need the center of the array to remain thus for the entire array. At the moment the array option kind of duplicates the segments but just throws them in position without anything keeping them there... which unfortunately means the next time I do anything the end up falling apart 😐

Another nice-to-have (although yes I am aware there are many work-arounds) would be for the 2 line segments (which in reality are one and the same line) to be constrained both collinearly and coincidentally at the end points. Unfortunately (so far as I can tell) the only way this can be done is manually?

Thanks again for taking the time with your example file 🙂

[Alfred.NESWADBA]

Hi,

I have not followed all these details, just want to verify that statement:

>> It is true that you cannot constrain the center

>> of an arc directly with AutoCAD's parametrics

For me, it works, at least how I understand "constraining center of an arc"

This is how it works on my side:

- alfred -

[Anonymous]

@beyoungjr

It was a difficult approach I would certainly agree but unfortunately so were all the others I attempted. A simple solution at this stage would run into more disruptive blockades later on in the process if not at that stage. I kept trying different approaches until unfortunately frustration got the better of me. Whilst the solution presented by @leeminardi is simple and works at this stage, as I demonstrated in my response it all falls apart when you want to add anything further to the model or modify it in any way.

Thanks for clarifying the history of the AutoCAD/Inventor, I was under the impression that AutoCAD was considered the far superior product when it came to drafting (although I'll admit I have my doubts). With that in mind I was expecting all the power and more of Inventor though definitely not the grace, your comments however seem to indicate I have incorrect information?

I'll try keep my posts brief in the future, I was simply trying to get it all down for reference.

[Anonymous]

@leeminardi

I was not aware of polylines not allowing the centerpoint reference (@Alfred.NESWADBA the question I had was regards this situation specifically, arcs are a different story entirely, they function as expected but thanks for your input :)). Do you know why this is the case? Presumably this behaviour is needed for some reason (or assistive in some way?). Interesting to note either way, I appreciate you letting me know.

Now having read your second comment I see your justification for the associative/not choice 😄 I hadn't read that far ahead yet, woops.

Your statement: "Instead, I used two lines segments that shared a coincident point and  a collinear constraint" has me puzzled somewhat. I thought that would be the logical next step in locking the shape in on the file you sent through but your statements seems to imply you had already done that? If you had it doesn't show up on my system unfortunately, are you able to clarify what you meant there?

[leeminardi]

@Alfred.NESWADBA  I stand corrected.  What mislead me was that when adding a dimensional constraint between the end of a line and the center of an arc is that when you click near the end of the line you will see the "X" in a red circle glyph at the end of the line indicating (to me) that a parametric point is being established while when you pick the arc (with osnap center) you only see the normal osnap center glyph. As you indicate, the center of the arc is in fact parametrically contrainted by the dimensional constraint.  Thank you for the clarification.  

[leeminardi]

Your statement: "Instead, I used two lines segments that shared a coincident point and  a collinear constraint" has me puzzled somewhat. I thought that would be the logical next step in locking the shape in on the file you sent through but your statements seems to imply you had already done that? If you had it doesn't show up on my system unfortunately, are you able to clarify what you meant there?

I've edited the colors of the base drawing (03) from my earlier post so that you can see that what looks like one red line is really two lines.  The red and green lines have a coincident point (at A) and a collinear constraint.  The same is true for the yellow and cyan lines (at B).  Two lines are used so that a vertex can be referenced and constrained by the 10.0 dimensional constraint.   The resulting geometry can be used in a polar array (non-associative recommended) to complete the design. 

I do not follow your statements about not being able to add additional constraints.  Please be specific and include an illustration.