topic Betreff: Add holes to a weldment in Fusion Support Forum

Add holes to a weldment

DonCMorrison — Sat, 29 Jun 2024 20:49:03 GMT

I have created a weldment with pairs of identical parts. I now want to add holes to just one of the parts without affecting the original components. How do I restrict the new features just to the weldment?

Betreff: Add holes to a weldment

g-andresen — Sat, 29 Jun 2024 22:07:38 GMT

Hi,

Please share the file for reply.

File > export > save as f3d on local drive > attach to post.

günther

Betreff: Add holes to a weldment

DonCMorrison — Sat, 29 Jun 2024 23:30:03 GMT

I have created the frame weldment as a component (without holes) and then inserted it into a new design and then tried drilling the holes, but fusion now tells me there is "no body selected)

Betreff: Add holes to a weldment

DonCMorrison — Sat, 29 Jun 2024 23:41:41 GMT

I am trying to model the parts as they will be made. No problem doing this in Inventor. Sorry if I'm being dense on this. My first try using the forum.

Betreff: Add holes to a weldment

jhackney1972 — Sun, 30 Jun 2024 00:43:22 GMT

If this is the hole, indicated by the red arrow, then you have an Externally Linked component, named Fold Frame. This component can be edit only with the Edit in Place option or by Breaking the external link. The one you choose depends on your Fusion License. If you have a Subscription then you can use the Edit in Place option, if not, you will have to Break the Link to the external model or edit the external model directly.

Betreff: Add holes to a weldment

DonCMorrison — Sun, 30 Jun 2024 01:45:44 GMT

So my problem is with the personal version of fusion. If I had the subscription would the edit in place edit just the Assembly that I have open or would it also change the linked version which is the welded version without holes? So far I am finding working with assemblies in fusion to be "highly illogical".

Betreff: Add holes to a weldment

DonCMorrison — Sun, 30 Jun 2024 01:59:13 GMT

The point is that I don't want to add the holes to the linked part. I want to add the holes only in the weldment. Makes sense to me but I guess not to everyone. Inventor has this capability but they have a weldment file type so I guess that would be more straight forward. Fusion does not recognize the concept of a weldment that is subsequently machined?

Betreff: Add holes to a weldment

jhackney1972 — Sun, 30 Jun 2024 11:28:08 GMT

With your license type you will probably be better off building your assembly with “local” components. This will allow you to add holes in your assembly as well as make better use of your ten active components restriction at one time. Right click on the linked external component and choose Break Link if you would like to use this method.

Betreff: Add holes to a weldment

Christoph_360 — Sun, 30 Jun 2024 16:07:13 GMT

Hello

If you use Insert Derive instead of Insert Component, you can modify the components in the new document.

(view in My Videos)

Mfg

Christoph

Betreff: Add holes to a weldment

Christoph_360 — Sun, 30 Jun 2024 16:17:19 GMT

Sorry @g-andresen, I wanted to send the message to @DonCMorrison of course.

Betreff: Add holes to a weldment

jhackney1972 — Sun, 30 Jun 2024 16:19:12 GMT

You are correct in the fact that you can add holes to a Derived file but in this case I think the original poster would be getting "a little deep" into his file dependencies. The Derive will be dependent on the assembly which contains an external reference to another assembly. Also, if he ever had to break the link on the derived assembly, in this case, he will be left with a lot of awkward base features.

Betreff: Add holes to a weldment

Christoph_360 — Mon, 01 Jul 2024 07:40:09 GMT

Hello

@jhackney1972 wrote:
You are correct in the fact that you can add holes to a Derived file but in this case I think the original poster would be getting "a little deep" into his file dependencies. The Derive will be dependent on the assembly which contains an external reference to another assembly. Also, if he ever had to break the link on the derived assembly, in this case, he will be left with a lot of awkward base features.

Yes, you're right, Insert Derive is not a sustainable solution for this task.

With a Configured Design and Insert Component, the task can be solved more sustainably.

(view in My Videos)

Mfg

Christoph