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Fitting multiple axis to a translated model where the translated holes have multiple faces

Question asked by David Whittaker on Apr 13, 2018
Latest reply on Apr 13, 2018 by Dustin Perreault

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Hoping someone has some brain wave which will help me.

I have multiple models which have come from a customer which when translated the holes come in with multiple faces which normally would be cylinders which I could easily put an axis on them by using the reference geometry axis command. I need to use the supplied models to extract geometry to get the cylinders or axis so I can transfer the holes into another part which can then be machined.

The only way I can think of is to put 3 points on the edge top and bottom, then putting a 3 point circle and a line between the 2 circles. The trouble is there are hundreds of holes and this would take forever and this is old data which there is no chance of replacing with more up to date data. Its all I've got.

An example of one of the models is attached and a screen dump of one of the holes showing the multiple faces

Yours hopefully

Dave

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96449-skin.SLDPRT.zip521.6 KB

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Tateos Tvapanyan Apr 13, 2018 6:44 AM
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It's not necessary to have a full circle to add reference geometry axis. Even a segment is enough to do it.
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- David Whittaker @ Tateos Tvapanyan on Apr 13, 2018 6:59 AM
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  Hi thanks for the reply, not on this model that's been translated. Its not seeing the segment as a true cylinder so wont let me put an axis on it. See the attached model and have a go
  Thanks
  Dave
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  - Tateos Tvapanyan @ David Whittaker on Apr 13, 2018 7:09 AM
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    Can you send me an IGES or xt files? I'm using SW16 and cant open already attached one.
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    - David Whittaker @ Tateos Tvapanyan on Apr 13, 2018 7:22 AM
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      Hi
      hopefully the models have attached to the reply.
      
      Thanks
      
      Dave
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      96449-skin.IGS.zip254.6 KB
      96449-skin.x_t.zip185.4 KB
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Brian Brazeau Apr 13, 2018 8:08 AM
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If you make a sketch on the face that has the holes on it you can use 3 point circle to make circles on each of the holes using the 3 points around each hole. Then that's all you need to make the axis because you can use face and point to make the axis. Still not much of a help, but at least you don't need 2 sketches for each hole. this is a case where patterning reference entities would come in handy.
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- David Whittaker @ Brian Brazeau on Apr 13, 2018 8:16 AM
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  Hi
  Thanks for your reply, that's one of my chosen methods at the moment with also putting a 3 point circle on each side and joining the 2 with a centreline its just that there are 100's of holes so is going to take ages.
  
  Dave
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  - Glenn Schroeder @ David Whittaker on Apr 13, 2018 8:25 AM
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    When you open the file, do you get a message asking if you want to use Feature Recognition? When I clicked yes, it took a while, but then they came in as cylindrical holes. I'd have saved it and posted it for you, but I'm using SW2018 so you wouldn't have been able to open it.
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    - David Whittaker @ Glenn Schroeder on Apr 13, 2018 9:18 AM
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      Hi
      
      Did all them get recognised as cylindrical holes ? When I try it doesn't see them all, it only sees about 6 as cylindrical holes. I'm using 2017.
      Could you save the model you create as a parasolid so I could open it and compare its result ?
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      - Glenn Schroeder @ David Whittaker on Apr 13, 2018 9:29 AM
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        David Whittaker wrote:
        
        Hi
        
        Did all them get recognised as cylindrical holes ? When I try it doesn't see them all, it only sees about 6 as cylindrical holes. I'm using 2017.
        Could you save the model you create as a parasolid so I could open it and compare its result ?
        
        I did have some weird graphics issues when I tried it. Some of the holes looked fine, and others would blink in and out as I manipulated the model. Oddly enough when I rotated it to the other side they all looked fine.
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- David Whittaker @ Brian Brazeau on Apr 13, 2018 8:29 AM
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  Now I've tried the method you just listed its not working its saying the point is outside the boundary ?
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  - Brian Brazeau @ David Whittaker on Apr 13, 2018 8:38 AM
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    Odd.It works for me SW 2016
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    - David Whittaker @ Brian Brazeau on Apr 13, 2018 8:49 AM
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      Did you use 3D sketch and pick 3 point circle and select end points to the sheet face which make up the cylinder ? How did you draw your circle to get the centre point ?
      
      Thanks
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      - Brian Brazeau @ David Whittaker on Apr 13, 2018 8:53 AM
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        didn't use 3D sketch. didn't have to face is a plane
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        David Whittaker @ Brian Brazeau on Apr 13, 2018 9:04 AM
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        That's curious the model I've got its not a flat face its original model is not flat its got a slight curve on it. Which model did you use out of the ones I up loaded ?
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        Brian Brazeau @ David Whittaker on Apr 13, 2018 9:29 AM
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        I used the parasolid x_t file
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Kevin Chandler Apr 13, 2018 8:32 AM
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Hello,

I tried recognize features on this to convert it, but automatic didn't translate all of the holes.
Interactive couldn't complete, but I was able to get them as outlined below:
1. Select the face and create an offset surface, zero thick
2. Thicken this surface and merge result
3. Save this file as an x_t parasolid
4. Import the parasolid and run recognize features (automatic)
  The original import geometry will be there along with a second one from your x_t export
  When prompted which to recognize, select the second one
It will chug for a bit, but the above is what came out of mine.
Cheers,

Kevin
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- David Whittaker @ Kevin Chandler on Apr 13, 2018 9:22 AM
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  Hi
  Ive just tried your method and on point 2 when thickening the surface the tick box for merge is ticked and it errors out, I have to untick merge for the thicken surface command to work. I then export or save the resultant thickened surface as a parasolid and import it and use the feature recog command and it only sees about 5 of them as holes
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Tateos Tvapanyan Apr 13, 2018 8:42 AM
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I did try the future recognize approach as Glenn Schroeder suggest and it gives the best result at the moment.
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- David Whittaker @ Tateos Tvapanyan on Apr 13, 2018 9:09 AM
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  Hi
  When you tried did it recognise all of them as holes ? it only sees about 5 as holes when I do it
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  - Brian Brazeau @ David Whittaker on Apr 13, 2018 9:49 AM
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    I tried the feature works method on the parasolid file and used interactive, chose only holes, and let it chug. I then used the find patterns and it found 7 linear patterns plus a few odd ball instances. I then rotated the part and saw the abnormality of partial skins over the holes. I used delete face with patch and got a clean looking model, but with a huge feature tree.(all the planes and hole features and delete face commands) I exported it as a parasolid then reimported it and saved as a solidworks doc. Nice clean doc and the holes are cylinders now.
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    96449-skin.SLDPRT.zip285.6 KB
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Dustin Perreault Apr 13, 2018 1:53 PM
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Here was my approach, using feature recognition seems to recognize and convert the holes but not through the entire part. You can see that one side has a strange thickness over the hole and the other is clear of the problem. I created a new sketch on the face using the convert entities command without problems and then extruded it to the original thickness. This is generally how I model though, using foreign solid bodies as a reference and recreating the model in a SolidWorks to have a new clean part. Doesn't take long at all. I would upload my file but I am using 2018.
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Fitting multiple axis to a translated model where the translated holes have multiple faces

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