topic Re: Cutting on component not working "No target body found to cut or intersect!" in Fusion Support Forum

Cutting on component not working "No target body found to cut or intersect!"

Anonymous — Fri, 20 Mar 2020 01:17:08 GMT

Hi,

I am not sure if this is possible in f360 or I am extrapolating naively from Inventor.

I am generating reusable components, each one put in its own file. Those files have usually one or at the most two bodies, they are very simple. I am working on a new file where I include the previously generated components to build an assembly.

To understand the picture better you have a C beam (80mm * 40mm and 3mm thickness) repeated 4 times to build a square frame. To be able to assemble this frame, each beam has 3 holes at each end, and a 8mm thick corner plate (290mm * 290mm) will be used for structural rigidity, by means of using bolts. The C beams are confronted on their flat side and separated 8mm which is the thickness of the corner plate. On purpose the plate has no holes yet. For now only one reinforcement plate is included in the assembly as I want to refine it with the respective holes first.

The rounded corners are to be more friendly with the laser cutter path and esthetics, and the slot is for hoisting.

The plate is "joint" in the assembly to fit where I want it to be and now I want to add the holes. The 3 growing complexity methods I tried unsuccessfully are:

1) Start a new sketch on the surface of the plate (I did it on both sides as somebody suggested it had to be done on the side of the original sketch side of the plate) and draw the circles myself by hand, closing the sketch and then do a CUT with the extrude tool.

2) Start a new sketch on the surface of the plate and be more refined and project the center of the holes of both beams on that new sketch. Then use those centers to draw the appropiate circles by hand, closing the sketch and then do a CUT with the extrude tool. This would enable future hole relocations on the beams to adjust if I do not break the link of the projected centers.

3) Do the same as 2) but project not only the center of the holes of the horizontal and vertical beam but the hole perimeter too. In this case I will inherit the position and diameter of the holes.

Here is a capture of the third method where 6 centers and 6 holes were projected.

My problem is that nothing of this has worked so far when I want to use that new created sketch in my naive conclusion it is referenced to the plate where the holes should be made.

The OK button never activates and I get the error message "Error: No target body found to cut or intersect!". I have tried with +10 and -10 and there is no change. I recall that a post was mentioning something about creating the sketch while the component was activated, but I cannot find a way to activate an external component and from all the reding came to the conclusion it is not possible?

Any hint if I am trying to stretch things or doing something wrong or missing a step. Or maybe there is a way to do this that does not follow this method?

Sorry for the long post and I have been reading on the issue the whole day with no success.

Regards

Thomas Magdahl (the subscription name does not match my name as it is a trial account of the company I am advising). We are evalauting if F360 is an option.

Re: Cutting on component not working "No target body found to cut or inters

jhackney1972 — Fri, 20 Mar 2020 01:37:05 GMT

Can you post your model so the forum users can work with it.

Re: Cutting on component not working "No target body found to cut or inters

davebYYPCU — Fri, 20 Mar 2020 02:01:51 GMT

You can not change a linked Component, in the Assembly file,

All those methods will work in it's own original file, or break this link.

You can derive the plate into this assembly, and make the holes, by all of those ways.

Your holes in a derived component will not link back to the original.

Might help....

Re: Cutting on component not working "No target body found to cut or inters

Anonymous — Fri, 20 Mar 2020 02:02:19 GMT

Hi jhackney1972

I have no idea how to do it. Would it be enough to attach the two component files and the assembly file?

Regards

Thomas

Re: Cutting on component not working "No target body found to cut or inters

Anonymous — Fri, 20 Mar 2020 02:08:49 GMT

Ok,

So either by breaking the link or creating the plate as a new component inside of the assembly I can use the projection method and then eventually save it to a file, but will loose the ability to update it dynamically when the beam holes change?

Regards,

Thomas

Re: Cutting on component not working "No target body found to cut or inters

davebYYPCU — Fri, 20 Mar 2020 02:16:59 GMT

I am more used to build in one file, and send DXF from it to Laser.

Are you looking for Configurations? Not yet in Fusion.

Might help...

Re: Cutting on component not working "No target body found to cut or inters

Anonymous — Fri, 20 Mar 2020 02:31:57 GMT

It seems I am trying to do things the "inventor" way by encapsulating as much as possible in separate files. And from all the reading, trying to figure this out and your input, I came to the conclusion that as much as possible, things had to stay in one file. I imagined that by creating a sketch on a surface of an external component in the assembly file, a new frame was created in that component file referenced or pointing to the assembly. In that way any change in the assembly would propagate to the component (obviously with the acceptance of the user). But I imagine this can originate circular dpendencies that would be a nigtmare to solve.

I do not know what "Configurations" are in the CAD world context.

Thanks for all your help! Should I mark the thread as resolved?

Regards

Thomas

Re: Cutting on component not working "No target body found to cut or intersect!"

Anonymous — Wed, 24 Mar 2021 22:24:20 GMT

Hi, I'm transitioning from Solidworks. To learn I am duplicating a design I currently have in SW and have run into a similar problem.

My method of modelling and file/part structuring is to mimic the production process. I begin with a generic base part. I then use it as the base component and machine it to create LH & RH parts in two separate 'assemblies'.

As per OP I can't get a cut until I do what is suggested here - break the link. This doesn't seem at all sensible because I want any changes in the base part to propagate through to the assemblies.

I have been a Professional Engineer using this design methodology for many years and its the standard for everywhere I've worked, both large and small. I'm sure that there must be a way to preserve the link but seeing as I'm unfamiliar with Fusion I'm sure I'm just looking in the wrong place/asking the wrong question. Thanks in advance for any tips.

Re: Cutting on component not working "No target body found to cut or intersect!"

davebYYPCU — Wed, 24 Mar 2021 22:44:56 GMT

You working with Fusion Rule No 1? Using the Timeline?

Each part in a separate component. Assembly of parts, developing cuts and tolerance from other components, is a normal workflow.

modifying a linked component in an Assembly, and expecting it to flow backwards, is not a normal workflow, but there is Edit in Place, these days, so maybe what you mean.

Might help....

Re: Cutting on component not working "No target body found to cut or intersect!"

Anonymous — Thu, 25 Mar 2021 01:57:36 GMT

Hi, thanks for the response.

>You working with Fusion Rule No 1? Using the Timeline?

Yes I am using the timeline. I've watched a lot of basics videos and transitioning from solidworks videos. I'm not coming at this blind and expecting the world to help me out 🙂

>Each part in a separate component.

Yes, I get that.

>Assembly of parts, developing cuts and tolerance from other components, is a normal workflow.

This (in bold) is the bit which isn't working and is what the question is about. Maybe I didn't make myself clear but the OP did make this clear so I thought that there was no point in my re-stating it exhaustively. The accepted answer in this thread suggests that developing cuts at assembly level is not possible and this what I'm sure can't be right.

>modifying a linked component in an Assembly, and expecting it to flow backwards, is not a normal workflow

Good. I don't expect it to flow backwards.

Maybe I wasn't clear enough. Consider this scenario:

I bring a generic part into an assembly and (within the assembly) engrave 'LH' in it to indicate it's the left of a pair.

If I open the generic part I don't expect it to have changed as a result of this.

If, however I open the generic part and change the thickness I expect the part in the assembly to update and reflect this thickness change.

I have been unable to make a cut at assembly level and I get the exact error as the title of this thread, hence my contributing here: "No target body found to cut or intersect!"

The advice here says that to be able to cut at assembly level you must unlink the generic part in the assembly from the generic part. And so if you change the generic you then have to manually change the assembly. Which doesn't seem right.

Re: Cutting on component not working "No target body found to cut or intersect!"

Anonymous — Thu, 25 Mar 2021 02:14:40 GMT

Here's a screenshot of what I mean and attached are the files so anyone can have a go at it themselves 🙂

Re: Cutting on component not working "No target body found to cut or intersect!"

jeff_strater — Thu, 25 Mar 2021 02:55:18 GMT

"If I open the generic part I don't expect it to have changed as a result of this.

If, however I open the generic part and change the thickness I expect the part in the assembly to update and reflect this thickness change."

I think what you are referring to are "assembly features". That is, a feature which affects a component, only in the context of the assembly, and do not affect the component itself. Fusion does not support assembly features.

Re: Cutting on component not working "No target body found to cut or intersect!"

taylorhsbennett — Thu, 25 Mar 2021 04:43:51 GMT

Forgive my lack of understanding please why are you are not just cutting out these holes to begin with based on sketch geometry then scale the parts . Do you need to have them cut at component stage for some reason . Let me know.

Re: Cutting on component not working "No target body found to cut or intersect!"

taylorhsbennett — Thu, 25 Mar 2021 04:50:10 GMT

I was able to create a plane on the side of a component using three points then draw a 3d sketch and then press pull out a circle in essence doing what you wanted.

Re: Cutting on component not working "No target body found to cut or intersect!"

taylorhsbennett — Thu, 25 Mar 2021 04:51:59 GMT

Solution :

Construct>Plane Through Three Points> Sketch geometry> Press Pull

Re: Cutting on component not working "No target body found to cut or intersect!"

taylorhsbennett — Thu, 25 Mar 2021 04:55:12 GMT

Make sure 3d sketch is selected in the options

Re: Cutting on component not working "No target body found to cut or intersect!"

davebYYPCU — Thu, 25 Mar 2021 05:11:52 GMT

Attach Your File.

Re: Cutting on component not working "No target body found to cut or intersect!"

Anonymous — Thu, 25 Mar 2021 21:56:29 GMT

>I think what you are referring to are "assembly features". That is, a feature which affects a component, only in the context of the assembly, and do not affect the component itself. Fusion does not support assembly features.

@jeff_strater Yes, that is exactly what I am referring to. I hope you are wrong that this is not supported because it's a massive part of the workflow for many types of manufactured part. It is very common to create generics then modify them at a later stage. However judging by your credentials I doubt that you are wrong.

Re: Cutting on component not working "No target body found to cut or intersect!"

Anonymous — Thu, 25 Mar 2021 22:14:25 GMT

Hi @taylorhsbennett

#1 Please consider finishing a thought before sending a new message. It makes things much easier to read.

#2 >Forgive my lack of understanding please why are you are not just cutting out these holes to begin with based on sketch geometry then scale the parts . Do you need to have them cut at component stage for some reason . Let me know.

I think you may be referring to the OP. In my situation I need the same base part and then different modifications based on if it goes on the LH or RH. My example with 'LH' is purely illustrational. Imagine it's a pivot for the suspension linkage on a car. You may want to attach something on different sides based on which side of the car it goes on. You wouldn't want a redundant hole so you modify the 'generic' to suit. As stated repeatedly, this is a very common situation for most jobs I've worked in.

#3 >Solution : Construct>Plane Through Three Points> Sketch geometry> Press Pull

Doesn't work for me. Please share a file with this geometry in it.

@davebYYPCU Are you asking me to attach my file or @taylorhsbennett to attach their solution? I believe I have attached my file.

Thanks all.

Re: Cutting on component not working "No target body found to cut or intersect!"

davebYYPCU — Thu, 25 Mar 2021 23:03:40 GMT

It was for @taylorhsbennett because he was contradicting us.

I think your best option is to investigate Derive.