Community
1976 Views, 17 Replies
When I tried to move EOP to extreme down following error message is coming. How to fix it?
@Anonymous
And what does the message state? Its right there (the reason why its failing) 
Mark Lancaster
& Autodesk Services MarketPlace Provider
Autodesk Inventor Certified Professional & not an Autodesk Employee
Likes is much appreciated if the information I have shared is helpful to you and/or others
Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Sketch5 has a repeated dimension and is missing a Tangent constraint.
Sketch8 has sick geometry (pink circle) that I assume was projected from a feature that was removed.
Did you remove a Ø.605 cylindrical feature or circle that existed earlier?
I notice that there is no Sketch 3, or 6. Did you use these sketches as parents and then delete them?
I notice that there are about 20 missing parameters.
Did you have a bit of trouble getting this far?
(There is nothing inherently wrong with having missing parameters - but from experience I associate this with a lot of fumbling around in creation of the geometry. You part is easily fixed by deleting the sick geometry or by deleting the projected constraint and re-dimensioning/constraining the circle.)
So, you learned that you can not playing with the eop as you like, but just when you strictly need.
The cause is.... shhhht happens, inventor (or other any cad programs) are not perfect, so, don't mess to much with it.
The other reason is... you're not perfect too, so, this is only one more step in your cad knowledge.
Solution: Try to repair all the mess caused by the "playing with the eop" and don't do it again, unless you stricly need to do so.
If you can't repair, do the part from the beggining.
CCarreiras
Hi fiatnm,
To fix the sketch you will want to right-click on the pink / magenta circle and choose Break Link, then you can dimension and constrain it in place, and update your feature.
Also, if it were me, I'd want Extrusion5 under Extrusion1. We typically want sketched base features first and then placed features (fillets, chamfers, patterns, shells, etc. ) last. That way you don't have sketches getting upset when placed features removed or updated.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
@Anonymous wrote:
Q1) Sketch5 has a repeated dimension and is missing a Tangent constraint.
A1) I don’t know which is repeated dimension. Target is for fully constraint sketch. Importance of inclusive of Tangent constraint is yet to be learned.
.... But I want to know why moving EOP was giving trouble.
Given that you can't find the repeated dimension (see image - I moved them closer together) - I am not sure you are ready for geometry constraints (like Tangent) or manipulating the EOP.
There were only 3 dimensions in the sketch? How is it not possible to recognize the repeated dimension?
Now, keep it simple..... is stupid??!! wow!!!! so wrong...
if you want to keep the KISS with some sense, try Keep It Super Simple, because stupid doesnt fit here at all...
CCarreiras
Hi fiatnm,
>> I wish to know what Break Link is doing behind the screen.
So when we project geometry, a link is created and the projected entity ( in this case a circle ) updates when the original geometry updates. But when the original geometry is no longer available, the projected geometry is "orphaned". Inventor gives us an error, and allows us to fix the sketch. Using the Break Link option makes the entity (again in this case the circle) independent, so that it behaves just as if you'd sketched it, rather than projecting it.
>> I follow your advice of 1st simple sketch and building on that and it is working well. Before I have to struggle many hours and many steps to get fully constraint sketch, now I can get it with a couple of steps.
Indeed the simple sketches method is extremely powerful, for beginners and experienced users both. When working in an office of professionals you are often required to update or modify someone else's work, and it can be very difficult to do when that work was created using sketches that contain geometry that controls multiple features. For that reason we prefer to see designs create models with the idea "how can model this so that someone else can update it quickly". Thinking about this as you model, saves time (and money) later.
>> Thank you very much for introducing simple method.
You're quite welcome, but I should point out that just as I have introduced this to you, others introduced it to me. I worked for many years using AutoCAD and am very proficient in that software. In it we "draw" rather than "sketch" and when I began using Solidworks and then Inventor, I was guilty of trying to draw complex sketches those softwares. Once I learned to use simple sketches, I was able to progress quickly learning the rest of the software since I didn't get stuck trying to create and modify sketches.
>> I have given a name for your method KISS (Keep it Simple and Stupid) approach.
I understand what you mean, as when we "dumb" down our sketches, it might make them seem less intelligent, since there is less information contained in them. But, I would say: Keep it Simple and Smart! , since when sketches begin to act stupid, it's often because the are not simple. Keeping them simple, keeps them acting smart.
Also, traditionally the KISS method means (Keep it Simple, Stupid!) , but in a professional business atmosphere the word "stupid" can be received poorly, offending others, and making them defensive, even when used as a joke, so we try to say (KISS = Keep it Simple, Sir!)
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
