Best way to repair micro gaps?

bruce_williams

Working with imported geometry, projecting silhouette to sketch with Use command.  Very small gaps at curve ends result.  Is there a way to avoid these and if not what is best way to repair?  The gap below is a sample it is 3.893e-5 in.  Once I have a good region, I want to extrude up to part to fill in below the silhouette so I am concerned I get a good enough match to do that.

1) Could just close with a line but that will create jogs.  And sometimes the end points are past each other...
2) Spend more time and move the end points farther apart (like .01") and patch with tangent spline.  More work but doable.

Hope clear enough without shared doc - it is proprietary.

.

owen_sparks

Hi @bruce_williams

I might:-

(i) Copy all the "used" entities onto a new sketch to kill all the use constraints in one go, and then add new coincident constraints where required to force them together.

(ii) Add some straight lines slashing across the whole sketch to chop up the regions to make identifying any gaps easier.  (Good bits filled in grey.)

(iii) Nag / encourage / bribe OS to add something to do this automatically.  The CAM software I use has such a feature.  You give it a tolerance dimension and then it'll join any points that are closer together than that value.  Runs in the blink of an eye.

Owen S.

emagdalenaC2i

1- You can show constraints and check if there are some missings coincident constraints, like in the upper left corner of this example
2- If you select all the entities with a box selection you can see if there are more entities than should be. Just take a look to the number next to the cursor

2- Then you can repeat the selection in a small part of the sketch to detect where are the extra entities

3 - You can press the right button and select "Select other..." to see all the overrlapping entities

4- Another test you can do is draw lines to see the created regions

5- You can also use the "Create selection" tool in the right menu and choose Edges --> Loop / Chain connected or Tangent connected

philip_thomas

@bruce_williams - As a pro user, we are here to help.
If you can't get it working, open a ticket and it will be assigned to an Engineer.

3dcad

This has been discussed few times earlier and as first cure Onshape should enable the possibility to box select endpoints for setting (coincident) constraint.
It is highly frustrating to zoom in and select point by point if there are say 100+ constraints to make.

@owen_sparks suggestion of automatic heal with tolerance would be perfect.

owen_sparks

Hi @bruce_williams

I might:-

(i) Copy all the "used" entities onto a new sketch to kill all the use constraints in one go, and then add new coincident constraints where required to force them together.

(ii) Add some straight lines slashing across the whole sketch to chop up the regions to make identifying any gaps easier.  (Good bits filled in grey.)

(iii) Nag / encourage / bribe OS to add something to do this automatically.  The CAM software I use has such a feature.  You give it a tolerance dimension and then it'll join any points that are closer together than that value.  Runs in the blink of an eye.

Owen S.

emagdalenaC2i

1- You can show constraints and check if there are some missings coincident constraints, like in the upper left corner of this example
2- If you select all the entities with a box selection you can see if there are more entities than should be. Just take a look to the number next to the cursor

2- Then you can repeat the selection in a small part of the sketch to detect where are the extra entities

3 - You can press the right button and select "Select other..." to see all the overrlapping entities

4- Another test you can do is draw lines to see the created regions

5- You can also use the "Create selection" tool in the right menu and choose Edges --> Loop / Chain connected or Tangent connected

bruce_williams

@emagdalenaC2C
@owen_sparks

Thank you both for some ideas I had not heard before.  I am going to work on this tomorrow and will report back.  I need to extrude up to the silhouette on free form part, so it will be interesting to see if can succeed with Onshape's limited surfacing & parting line tools.

philip_thomas

@bruce_williams - As a pro user, we are here to help.
If you can't get it working, open a ticket and it will be assigned to an Engineer.

bruce_williams

Success!

@emagdalenaC2C 
1) Great tips on getting a count of number of entities.  Let's you find where things are doubled up.
2) I have used the line 'slashes' and that continues to be the best way to find open geometry.  
3) Looking for missing constraints is good also.

@owen_sparks 
Your suggestion to get rid of Use constraints and add Coincident was the solution for me.

Once I had closed geometry, I just offset it in .001" and then it would extrude up to part just under the silhouette (parting line).

Still a ways to go; I hope to grab the edge of the faces into a Composite curve to effectively have a parting line curve.  Then I will create a loft below that for draft.

emagdalenaC2i

I'm glad to know that it worked for you

3dcad

This has been discussed few times earlier and as first cure Onshape should enable the possibility to box select endpoints for setting (coincident) constraint.
It is highly frustrating to zoom in and select point by point if there are say 100+ constraints to make.

@owen_sparks suggestion of automatic heal with tolerance would be perfect.

emagdalenaC2i

I made an application many years ago for the design and cutting of stone facades on AutoCAD which included a series of tools to detect basically all the errors you mentioned and many more.

I'm not sure if I could use FeatureScript to traverse all the entities of an existing sketch, but if I can ... It would be an interesting project to do the migration of this old AutoLISP code to FeatureScript ;-)