Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Pocket Operation For Vacuum Bed

33 REPLIES 33
Reply
Message 1 of 34
richardlaney
845 Views, 33 Replies

Pocket Operation For Vacuum Bed

Hi, have read some similar posts and responses but still somewhat unclear on the solution. 

 

I have made a simple vacuum bed with 8x8mm channels (slots). The design was made using ‘mirror' instead of ‘pattern' in the drawing phase. 

 

Fig:1 

 

Screenshot 2024-03-11 at 11.52.42.png

 

I am attempting to use a ‘2d pocket’ operation to cut out the channels (using a 6mm bit). 

 

The issue I’m having is I can't get the tool to stay down. If I select the base of the 8mm slot, it recognises it but then wants to helix back in, on every extruded island.

I cannot get it to see the entire floor as one big pocket with islands. It seems to instead recognise the islands and wants to cut them out individually. 

 

Fig: 2

 

Screenshot 2024-03-11 at 11.57.25.png

 

What I’m trying to achieve is the most efficient way to machine this. Helix'ing into over 100 islands can’t be it?

   

Help much appreciated. 

33 REPLIES 33
Message 2 of 34
richardlaney
in reply to: richardlaney

Here are some pics of my Pocket setup. 

 

Screenshot 2024-03-11 at 12.10.34.png

 

Screenshot 2024-03-11 at 12.12.39.png

 

Screenshot 2024-03-11 at 12.13.07.png

 

Screenshot 2024-03-11 at 12.13.21.png

 

Message 3 of 34
seth.madore
in reply to: richardlaney

Would you be able to share your Fusion file here?
File > Export > Save to local folder, return to thread and attach the .f3d/.f3z file in your reply.

 

I'd be looking to program up a few islands (or maybe one strip of them) and then using Pattern > Duplication to propagate the CAM features across the rest of the part.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 4 of 34
richardlaney
in reply to: seth.madore

Hi Seth 

 

Here is the file. 

 

 

Message 5 of 34

An 8mm wide slot with a 6mm bit. I see that you have left the maximum stay down distance too 1500mm but won't the 3mm safe distance prevent the tool from staying down when there's is only 0,5mm of available clearance in the slot? 

Message 6 of 34

You'll have to excuse my ignorance. I'm relatively new to CAD and self taught. Trying to understand Fusion 360's CAM is proving difficult. 

 

I'm using a 6mm bit because I wanted some slight compression in the corners, so the gasket has a snugger fit. When I did an 8mm radius in the corners, the gasket seemed to have more room around it, likely due it being under its own compression. It might not be needed but it's a bit of trial and error. 

 

Regarding the safe distance, there are many little things in Fusion CAM that do not make sense to me. Whether it's the nomenclature used and or the description, it's still not clear to me what the feature is doing. 

I have yet to find some material that explains these little things in language that makes sense to me. 

 

I don't understand what the 'safe distance' means and I don't understand how there is 0.5mm left in the slot?

Could you explain further?


Cheers. 

Message 7 of 34
richardlaney
in reply to: seth.madore

Hi Seth

 

Sorry if you could, can you describe in more detail what you mean by 'program up a few islands'?

That's not something I'm familiar with doing or quite understand what you mean. 

 

Many Thanks. 

Message 8 of 34
seth.madore
in reply to: richardlaney

Sure thing, looking at your file now. Will be back with some advice!


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 34
seth.madore
in reply to: richardlaney

First off; what is the material for this and what is your machine? I'm waiting for Adaptive to calculate, and 50 minutes in, I'm getting rather impatient....


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 10 of 34
seth.madore
in reply to: richardlaney

Here's how I would approach it if it were me:

2D Contour to rough out a bunch, 3D Pocket Clearing to finish the rest of it:

2024-03-12_07h38_28.png


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 34
richardlaney
in reply to: seth.madore

The material is PE500 but I have not specified anything in Fusion. 

I should recheck my cutter specs but I think it's Feeds and speeds for MDF. 

 

My machine is a CNC router with a 2.2kw spindle and a steel frame. A bit more robust than the average hobby machine  

but not a professional level machine.

 

You'll have to excuse my lack of knowledge Seth, I'm self taught and not very knowledgeable with CAM. I have been machining for nearly 2 years now  and thankfully have managed to get on quite well. No crashes yet! 

There are however basic things I still haven't grasped.

 

I'll have a look at the file now and report back. 

Message 12 of 34
seth.madore
in reply to: richardlaney


@richardlaney wrote:

You'll have to excuse my lack of knowledge Seth, I'm self taught and not very knowledgeable with CAM. I have been machining for nearly 2 years now  and thankfully have managed to get on quite well. No crashes yet! 

There are however basic things I still haven't grasped.

 


No apologies needed, at all. We all start somewhere and we're grateful you've come to the forum to seek help!

 

Regarding the material and speeds and feeds; Fusion does not yet have the ability to calculate speeds/feeds based on material, it's all up the user to determine what is best for their needs.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 13 of 34
richardlaney
in reply to: seth.madore

Seth thankyou for making me feel welcome and your support.

 

Had a look at the file, looks great. I've gone over the details of your methods and they seem to fall very much in line with proper CAM machining. Usually when I'm machining and because I'm not machining in metal, I do not bother with stock to leave, or smoothing operations, which I assume are really important when it comes to getting a good finish in milling metals etc.. 

 

I had two questions about your strategy. 

 

1) When ramping @10 degrees for the '2D contour' is it preferable  (I assume it is hence why you did it), to continuously ramp? I've preferred (likely through lack of knowledge), to have a short ramp and then a flat cut at required depth, for tool efficiency and speed, due to ramping operations usually being slower than normal cutting. Thoughts? 

 

2) Do you agree that it would be better for me to change the cutter to an 8mm, for the 'Pattern' operations. It would speed up both that and make the final operation unnecessary. Of course you have worked with what I've given you. I'm very impressed with how you managed to keep the tool down in the final pocket operation. That was what I was hoping to achieve and spent several days trying. 

 

Should have reached out sooner. 

 

Let me try to CAM that and send it to you. See if I've managed to progress here! 

Message 14 of 34
seth.madore
in reply to: richardlaney

1) Not knowing the material or "stoutness" of your machine, I opted to stay on the conservative side. If it was being run on a beast of a commercial machine, I'd likely do a short zig-zag to depth and just zip around it.

2) As I trend towards the conservative side of things in many areas of life, my approach to machining is much the same; I prefer Stock to Leave and gentle finish cuts. Smoothing, on the other hand, is not something I would consider optional, as it will often result in a much smoother processing of code (this is usually a function of the code processing speed of the controller). Without Smoothing turned on, you may find that the machine is stuttering in some areas and not even reaching the speeds you've defined.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 15 of 34
richardlaney
in reply to: richardlaney

Seth is the last pocket operation you used, a custom one?

There is no 2D or 3D designation given in the tab. 

 

When doing the linear 'pattern' operation, I notice the tool plunges at the end of the travel to go down a level. I was told plunging is to be avoided if possible but I notice that the 'pattern' parameters do not give any real choice?

 

 

Screenshot 2024-03-12 131809.png

 

 

Message 16 of 34
seth.madore
in reply to: richardlaney

The last toolpath is known as "Pocket Clearing"  found in the 3D tab:

2024-03-12_09h29_20.png

If you notice, my first toolpath is a 2D Contour that zips around the outside, which gives us the clearance needed for 2D Contour (with Both Ways and Plunge) to enter and exit into open area.

Yes, in general, plunging directly into material is to be avoided.

 

Regarding the Patterns; to use these, we first create a toolpath with the conditions we prefer. Once we are pleased with the result, we can right click on the toolpath and "Add to new Pattern".

2024-03-12_09h32_32.png

 

That Pattern will just duplicate/Transform based on settings of the Pattern, replicating that exact toolpath many times over (based on settings of Pattern)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 17 of 34
richardlaney
in reply to: seth.madore

Ah yes I see, the contour allows for further plunges. I understood the initial plunge but didn't pick up on the subsequent ones. Very clever! 👌

 

My understanding of your approach is that you

 

1) Initially cleared the outer perimeter to allow for the 'Pattern' operation to plunge.

2) You '2D pocket' cut the hollow areas (they will be cut later to allow for ducting). I assume this is just better to do now than later, whilst you have more meat to cut into? 

3) You pattern a tool path to create the channels but I am unsure as to why you didn't clear those channels up whilst in that operation? I thought the 'pattern' operation is in and of itself, a defined cutting operation but it is instead a method applied to a defined operation? Am I to assume then the the underlying operation is 'slot', which you then patterned?

 

Two questions:

  1. Is that why you did not clear the channels to the desired width because you were using a slotting operation that cuts a single line?
  2. How did you find a centre line to slot to? Did you create a sketch line in 'design' and then use it to define the 'slot' pathway? I do have some centre lines of course in the design but I'm not aware that you can see sketch lines in CAM.

 

4) You then go back over it all with a pocket clearing operation, to remove remaining stock which you helix into and then cut per step down. 

I'm not sure how you managed to keep the tool down here and the nuances between '2d Pocket' and 'Pocket Clearing'.

I'm assuming that your ability to keep the tool down is partly based on the 'Pocket Clearing' but that you had already gone down to depth with the 'pattern' operation, which therefore allowed the 'pocket clearing' to create a more efficient path?   

 

 

Message 18 of 34
seth.madore
in reply to: richardlaney


@richardlaney wrote:

My understanding of your approach is that you

 

1) Initially cleared the outer perimeter to allow for the 'Pattern' operation to plunge.

2) You '2D pocket' cut the hollow areas (they will be cut later to allow for ducting). I assume this is just better to do now than later, whilst you have more meat to cut into? 

3) You pattern a tool path to create the channels but I am unsure as to why you didn't clear those channels up whilst in that operation? I thought the 'pattern' operation is in and of itself, a defined cutting operation but it is instead a method applied to a defined operation? Am I to assume then the the underlying operation is 'slot', which you then patterned?

4) You then go back over it all with a pocket clearing operation, to remove remaining stock which you helix into and then cut per step down. 

I'm not sure how you managed to keep the tool down here and the nuances between '2d Pocket' and 'Pocket Clearing'. 

I'll have a play around with it and see if I can get more familiar. 

 


1) Correct

2) Cuz it struck my fancy, no other reason

3) We could have, but your islands have radii on them, we'd be going back in there anyway. Based on my prior comment about approaching machining in a conservative fashion, it's "how I roll".

3a) No, not the Slot toolpath, I just used 2D Contour and turned on Stock to Leave of 1mm. Since the tool is 6mm, and the slot is 8mm, 1mm puts this tool smack dab in the middle of the slot

4) In the Pocket Clearing (and other) toolpaths, there's a Max Staydown distance. I set it to something large (2000mm I think) and that allowed it to navigate around with the tool staying down.

 

The difference between Pocket Clearing and 2D Pocket are rather massive: Pocket Clearing is "model aware", 2D Pocket is not, requiring instead manual or semi automatic selection of geometry. I opted to maintain the depths of cut in Pocket Clearing, as I didn't know quite what scenario you were faced with. You could set Max Stepdown to something larger and just avoid the Stepdowns altogether. Another option, if you want to avoid the steps altogether is to instead use the Flat toolpath, although I think there may be much more linking and repositioning going on with that toolpath...


@richardlaney wrote:

Two questions:

  1. Is that why you did not clear the channels to the desired width because you were using a slotting operation that cuts a single line?
  2. How did you find a centre line to slot to? Did you create a sketch line in 'design' and then use it to define the 'slot' pathway? I do have some centre lines of course in the design but I'm not aware that you can see sketch lines in CAM.

 

 


1) See response to #3

2) See 3a


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 19 of 34
richardlaney
in reply to: seth.madore

- "3) We could have, but your islands have radii on them, we'd be going back in there anyway"

- Yep makes sense now. 

 

- " 3a) No, not the Slot toolpath, I just used 2D Contour and turned on Stock to Leave of 1mm. Since the tool is 6mm, and the slot is 8mm, 1mm puts this tool smack dab in the middle of the slot".

- Ok got it!

 

- "4) In the Pocket Clearing (and other) toolpaths, there's a Max Staydown distance. I set it to something large (2000mm I think) and that allowed it to navigate around with the tool staying down."

- I've often tried to use 'staydown' but it has never worked in keeping the tool down. As shown in the original file CAM

 

"You could set Max Stepdown to something larger and just avoid the Stepdowns altogether".

- I usually try to go in 3-4mm stepdowns to go easy on the tool and machine. I had noticed yours and thought they were in line with what I usually do so no problems there. 

 

" if you want to avoid the steps altogether is to instead use the Flat toolpath, although I think there may be much more linking"

- I'm going to save that option for another day but thanks for suggesting it. 

 

 

I'm going to try to rebuild your CAM from the ground up and see if I can arrive at the same place. Best way to learn is to internalise. I've taken a screen shot of all the data in case I get stuck. I know you can save the strategies as templates but that would be cheating.

 

Perhaps then we can look at using an 8mm bit and see if it drastically improves the machining time? I think the current one clocks in at about 1:20hr

 

One thing that does throw me off is that in 'heights' if you select 'selected contours', it doesn't show the depth to which the machine will cut and so you automatically think it isn't going to cut anything. 

Message 20 of 34
richardlaney
in reply to: seth.madore

Seth can't figure out how you managed to do the 2d pocket 'closed chains'. 

 

I've had a peak at your method but it doesn't get me there for some reason. 

 

You select 'chain' then 'sketch segment'.

 

Screenshot 2024-03-12 164835.png

 

I don't get the option to choose 'Sketch Segment'. 

 

Screenshot 2024-03-12 164851.png

 

 

So I am unable to replicate your strategy.

Can you go through how you were able to create this 👇

 

Screenshot 2024-03-12 165620.png

 

 

Seth ignore this message, I've figured it out. I had no idea you could view sketches in 'Manufacturing'. Amazing how I got this far really! 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums