AnsweredAssumed Answered

Can't figure out what to edit to change this hole pattern

Question asked by Stephen Wilson on Apr 29, 2020
Latest reply on Apr 29, 2020 by Glenn Schroeder

Like • Show 0 Likes0
Comment • 6

I'm modifying a part made by someone else. I want to change the location of the "7.0 Diameter Hole". If I'm not doing a linear pattern, I typically make a sketch with points first, and then use the location feature in the hole wizard to place them on the points so if I want to change the placement of the holes I can just change the dimensions of the points.

But when I use the edit feature or edit sketch commands in the feature tree, I cannot find any dimensions to modify. Either I'm missing something obvious or the designer did this in a way I'm not familiar with.

I have included the file also, if anybody can tell me what I'm missing.

Thanks in advance for your time.

Dan Pihlaja Apr 29, 2020 4:40 PM

Correct Answer

This was created in context inside an assembly:

You have 2 options:

1) open that assembly and edit whatever those holes are concentric to.

Here:

2) Delete all the concentric constraints and create your own. Then edit as needed.

Warning: This will break the link to the assembly. You should know if that is indeed what you want before you do it.

See the reply in context

Attachments

7.0 Hole Pattern.SLDPRT.zip131.0 KB

No one else had this question

Outcomes

Josh Brady Apr 29, 2020 4:38 PM

You are missing a couple of things. One of which is "Power Supply.SLDASM"

Actions

Dan Pihlaja Apr 29, 2020 4:40 PM

This was created in context inside an assembly:

You have 2 options:

1) open that assembly and edit whatever those holes are concentric to.

Here:

2) Delete all the concentric constraints and create your own. Then edit as needed.

Warning: This will break the link to the assembly. You should know if that is indeed what you want before you do it.

Actions

Stephen Wilson @ Dan Pihlaja on Apr 29, 2020 4:41 PM

Ah! I understand now. Got it! thanks.

Actions

Heiko Sohnholz Apr 29, 2020 4:39 PM

Hi,

as you can see, there are some arrows in the feature tree ( ->? )

This means, that this part has external references to other parts. So it might get the positions over the assembly from another part or sketch. Right click on the sketch and look for these references, and you will see.

Do you have the complete assy? If yes - open it up and change the referenced part. This is because the bore positions should match (of course!)

Actions

Stephen Wilson @ Heiko Sohnholz on Apr 29, 2020 4:41 PM

Got it! Thank you.

Actions

Glenn Schroeder Apr 29, 2020 4:44 PM

It looks like this Part was edited inside an Assembly, and those points were placed concentric with features in another Part, but it's easy enough to fix. Here's what I'd do:

Pull the rollback bar up just above this Hole Wizard feature.
Create a sketch to drive the Hole Wizard locations, just like you'd normally do for a new Hole Wizard feature.
Pull the rollback bar back down.
Expand the Hole Wizard feature in the tree.
Click on Sketch4- in the tree and choose the "Edit sketch" icon.
Delete the relations driving the locations of the points and re-apply relations to your sketch. You could probably just delete all these points and insert new ones, but if this Part is used in an Assembly that would probably cause mate errors.
Exit the sketch and it should be fixed.

Edit: I see I was late to the party. That's what I get for giving so much detail.

Actions

6 Replies

Josh Brady Apr 29, 2020 4:38 PM
Mark Correct
Correct Answer
You are missing a couple of things. One of which is "Power Supply.SLDASM"
Like • Show 0 Likes0
Actions
Dan Pihlaja Apr 29, 2020 4:40 PM
Unmark Correct
Correct Answer
This was created in context inside an assembly:

You have 2 options:

1) open that assembly and edit whatever those holes are concentric to.
Here:

2) Delete all the concentric constraints and create your own. Then edit as needed.
Warning: This will break the link to the assembly. You should know if that is indeed what you want before you do it.
Like • Show 2 Likes2
Actions
- Stephen Wilson @ Dan Pihlaja on Apr 29, 2020 4:41 PM
  Mark Correct
  Correct Answer
  Ah! I understand now. Got it! thanks.
  Like • Show 1 Like1
  Actions
Heiko Sohnholz Apr 29, 2020 4:39 PM
Mark Correct
Correct Answer
Hi,
as you can see, there are some arrows in the feature tree ( ->? )
This means, that this part has external references to other parts. So it might get the positions over the assembly from another part or sketch. Right click on the sketch and look for these references, and you will see.
Do you have the complete assy? If yes - open it up and change the referenced part. This is because the bore positions should match (of course!)
Like • Show 0 Likes0
Actions
- Stephen Wilson @ Heiko Sohnholz on Apr 29, 2020 4:41 PM
  Mark Correct
  Correct Answer
  Got it! Thank you.
  Like • Show 1 Like1
  Actions
Glenn Schroeder Apr 29, 2020 4:44 PM
Mark Correct
Correct Answer
It looks like this Part was edited inside an Assembly, and those points were placed concentric with features in another Part, but it's easy enough to fix. Here's what I'd do:
1. Pull the rollback bar up just above this Hole Wizard feature.
2. Create a sketch to drive the Hole Wizard locations, just like you'd normally do for a new Hole Wizard feature.
3. Pull the rollback bar back down.
4. Expand the Hole Wizard feature in the tree.
5. Click on Sketch4- in the tree and choose the "Edit sketch" icon.
6. Delete the relations driving the locations of the points and re-apply relations to your sketch. You could probably just delete all these points and insert new ones, but if this Part is used in an Assembly that would probably cause mate errors.
7. Exit the sketch and it should be fixed.
Edit: I see I was late to the party. That's what I get for giving so much detail.
Like • Show 2 Likes2
Actions

Can't figure out what to edit to change this hole pattern

Attachments

Outcomes

Related Content

Recommended Content