Problem with a smart component

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1

Hello everyone,

I have a problem with a smart component, I have 4 holes to make using a single function, when I make 2 holes it works, but when I make 3 or 4 I have an error visible in the attached image.

I don't understand why it doesn't work when it's so simple to use in principle.

Thanks in advance

 


erreur.png
2

Hello

 

For my part, I don't use the part where we select the components because I don't represent the screws and therefore I only have the plan to select.

Basically for the material removal function I have 4 circles, at the diameter of the digital one, in the same sketch.

Of course, if your model has several configurations, with a number of screws that changes and depth that also changes, it gets complicated.

Which version of SW are you on? (I can only send you a 2019 version as an example)

3

Hello

Can you attach a picture of the corresponding "Enlev.nat.Extru2@dessous" image of the corresponding sketch and material removal. (It is possible that it comes from there.)

Also make an image in the feature manager of "smart functions" (Folder with a star)

Kind regards

4

Thank you FUZ3D for your answer,

Yes, that's exactly what I did with the extra screws and yes I have several configurations but only according to the height of the legs.

I'm in the 2018 version

5

That's Zozo_mp

 

I put the first  picture on you.


enlevement_matiere.png
6

And here is the second


fonction_intel.png
7

If your function has the 4 holes try without selecting the screws to see if it works like that. as for the depth if they are pointings you might as well leave a Z-3mm whatever the screws are, right? or if you go through a 2d DWG the depth is determined by the one who is machining.

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8

I don't have any better without the screws, I have the same message and suddenly no intelligent function is created.

Otherwise quite a 3mm pointing suits me very well (program generation from swoodCam).

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9

I tried it again and always the same message.

Any idea?


fonction_intel2.png
10

Is it possible for you to join us your assembly to see if I can find out what's wrong. (I don't rule out a whim of SW^^)

90% of my Intel parts are made to create holes for handles or clasps and therefore is limited to drilling / routing in panels.

In your tree we can see that this is the right function: here is one of my examples with 2 functions (1 for drilling and the other for routing), so I don't see any reason why it shouldn't work for you.

NB: by the way, I take this opportunity to say in a general way that the part / panels that serves as a support have a unique name (do not leave room 1 for example) otherwise you risk having conflicts between all your intel and SW parts is lost as a result.

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11

Hello@fuz3D

Question: if you have a hole of Ø 4 and you want to put a function with a  Ø 6 it works.

Because @treza88 put Ø3 holes and at the beginning there weren't even holes if I read correctly.

Kind regards

PS: @fuz3D says  """90% of my intel parts are made ""  it's Intel In Side"""    ;-)  ;-) ;-)

12

@Zozo yes yes of the intel Xeon :p

To come back to using the intel parts the most annoying is to manage the diameters and therefore not sure that it follows as it should, (personally we work with rivet so 5.2mm drilling in all cases, same for the number of holes I don't know how to vary it, on the other hand if the position is different between the different configurations of the part it's Yes.

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13

Here is my assembly file


assemblage15.zip
14

Well, I found, it's just the way you created your score nothing dramatic.

Remove the coincident constraint is what creates a link that SW obviously doesn't like.

Use an entity conversion of your 5mm hole and then make a concentric with the 3.5mm one.

Or another variant make the circle of the pointing on the base part and have the entity of the sketch converted (practical when there are several holes)

The only bug for the latter is that from time to time SW displays the sketch of the pointing instead of keeping it hidden. (opening and closing the part is enough to remove it from the assembly)

 

(EDIT: Loss of image)

15

Here is the corrected version in its version 1 (3.5mm circle on the part that receives)

 

16

I'm sorry, but I'm really bad at it, I can't do an entity conversion after editing my base panel.

I don't have to do it right.

17

Create your sketch on the panel, then select the circle of the 5mm parking and then entity conversion.

Then pass it in construction, then make a 2nd circle of 3mm and finish with extrusion (which is already present, if not create it)

18

I have just taken your step, if I am not mistaken.

It works, on the other hand if I haven't messed up, I end up with a sketch alone containing the 5mm circle obtained with convert entities which does not belong to a part but to the assembly.

Is that right or should the sketch be in a room?

19

I think that the 2 cases work, personally I do on the part and no extrusion in assembly. As long as it works, that's the main thing.

20

Ok anyway a big thank you for your help, because before finding where the subtle error came from, I could spend a moment there.