Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

how to avoid stock collisions ? can't seem to get control over this.

rumpelstielz
Collaborator

how to avoid stock collisions ? can't seem to get control over this.

rumpelstielz
Collaborator
Collaborator

hi all, just finished my last project but once again i was battling with the settings for adaptive operations where i can't seem to get rid of stock collisions. If you look at the attached file you'll see shedloads of 'collision with stock' all over the place.

 

To be honest i can't figure out why this is happening and more specifically why Fusion is not taking care of this on it's own since there doesn't seem to be a logical explanation as to why Fusion sets the toolpaths like this, most of the time the moves that generate the colissions seem to be totally avoidable within the machines movements. I've been working with Rhinocam for the last 4 years and to be honest this has never been an issue before, unless i do something unbelievably stupid in the toolpath settings i can more or less let the machine run without having to worry that a bit will break or my stock gets ripped out of the fixtures because the bit is plunging or running into unmachined stock at random intervals.

 

Although i managed to finish the part with the CAM settings in the file posted i was literally sitting through the whole thing next to the machine nursing it, turning up the spindle speed when the machine was ploughing through too much stock unexpectedly (my machine has a very weak spindle and turning up the speed helps get through more stock sometimes).

 

So what's the deal here ? Why is Fusion setting toolpaths that potentially can ruin a part, break bits, or if this was metal even break the machine ??? An more importantly, how do i get control over this, as it is machining becomes a risky guesswork. I've literally spent days playing around with all possible option but i cannot get precise control over this operation.

 

Of course there might be several other ways to roughmachine this part to prepare for a parallel or contour finish, but the point here is that i cannot figure out how to get rid of the rapid stock collisions at all, no matter what i do. Everytime i try using adaptive (which is my preferred roughing method since my old machine handles it very well and it tends to run smoother than say a 3d pocket operation). I read through all the documentation and searched the forums but could not find a solutions to this.

 

any help towards understanding the source and possible solutions to this would be much appreciated

==================================================
GENERAL DISCLAIMER: if there isn't a file attached to my posts then there is a reason for it. wherever i can i will attach a file for troubleshooting.If no file is attached i will always try to explain as clearly as possible with illustrative screenshots. when i have an issue that can only be helped by attaching a file which i cannot share publicly i won't ask about it here.
0 Likes
Reply
2,893 Views
8 Replies
Replies (8)

LibertyMachine
Mentor
Mentor

Ok, long winded response below. Sorry in advance for the wall of text...

 

So, normally when I open up someones file that they have shared, I generally figure out what they are trying to accomplish and find the one or 2 spots that they have had issues with.

Your file has presented a few more challenges than normal. When I first opened it up, it wasn't displaying the stock in Simulation mode. That puzzled me for a moment, until I realized that in your Setup, you didn't have any stock selected. It was set to "From Solid" but nothing was selected. Not sure if that was intentional, or something that got messed up in the export... That aside, let's start at T1, the 3mm endmill. You have collisions with that tool because the flutes are not long enough, on the 3rd drilling operation. Curious, why do you have 3 different drill operations using the same holes?

Next, onto the 3D Adaptive. There were several things here that I would like to improve upon, if you don't mind. I'll take it through one operation tab at a time:

Geometry tab: You can leave it set to Silhouette if you want, or you can set it to Profile. Setting it to None will machine the entire part, stock included. Are you using bolts through the part to restrain it? If so, you don't want it set to None, as that will clear those out. Best bet would be to set it to Silhouette or Profile, Tool Outside Boundary as well as an Additional Offset of at least half the tool diameter.

Stock Contours. These really need to be turned on if you are trying to avoid crashing into stock. This is pretty much the main way you control how it "knows" where stock is. So, turn it on and select the profile of the stock you have modeled.

Model(s): Leave this field blank. The only thing it really is doing for you is increasing processing time. The Model is already selected in the Setup, so it's not going to cut through it by accident (assuming things are set proper). I know you are thinking that will control where the tool cuts, but that's not how it works. Hovering over the Model button gives you no info, and that's a shame. I think it's related to having multiple models in the setup, but I'm not certain. More info here would be nice. All I can say is that I never have to select anything at that point

 

Heights: Not a lot to say here, other than I notice that your WCS is way out in space and I wonder if that's intentional or.....? For bottom height you are saying "Model Bottom" plus another 3.9mm offset. Where does that put you on the part? Alternatively, you could also use Selection and select a face. It may be easier in the long run

 

Passes: Maximum Roughing Stepdown set to .5mm. Are you sure that's necessary? You posted a video the other day of how poor the simulation performance was. I see why now... .5mm stepdown is EXTREMELY light. More appropriate would be a rough step of .250" and a Fine Stepdown of .025"

 

Linking: And here is where a LOT of your collisions were coming from. You had the entry set to Plunge. That will drive the tool into the part at full rapid. You really should set it to Helix, if you are starting in the part. I'd also want to increase the Max Stay Down distance to a more realistic value, such as 1-2", that will reduce the amount of up/down that you would see

 

So, in closing, I've attached your file with a few changes that I would be inclined to do.  Of course, I don't know the material you are working with, the rigity of your machine or even how you plan on holding this part.

 

I didn't go all out and look at every operation, just more the 3D adaptive. If you have ANY further questions, don't hesitate to ask

 


Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
2 Likes

HughesTooling
Consultant
Consultant

@Anonymous wrote:

Model(s): Leave this field blank. The only thing it really is doing for you is increasing processing time. The Model is already selected in the Setup, so it's not going to cut through it by accident (assuming things are set proper). I know you are thinking that will control where the tool cuts, but that's not how it works. Hovering over the Model button gives you no info, and that's a shame. I think it's related to having multiple models in the setup, but I'm not certain. More info here would be nice. All I can say is that I never have to select anything at that point

 


 

I made a screencast a while ago to show someone when and how to use Model selection in an op, they were misusing it to contain toolpaths. The part had some engraving and this made the toolpath uneven, selecting a patch and include setup model covers the pockets made by the engraving and give a far better toolpath.

 

 

Mark

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


3 Likes

LibertyMachine
Mentor
Mentor

Thank you sir. I had seen that screencast when you shared it a while back, but it didn't register in my mind the depth you were going into. Thank you for bringing it back up. Have you found any official "best practices" guidelines, or has this been trial and error on your part?


Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
0 Likes

HughesTooling
Consultant
Consultant

There doesn't seem to to be anything in the help anywhere, I have asked for a quick tips video to be made. There was a request from someone on the support team for ideas for quit tip videos and I pointed them to the thread I made the screencast for, they seemed quite enthusiastic especially as the thread showed up the problem so well. I made the same mistake when I started using Fusion, back then there was no auto select in the setup so it was even more of a problem, I think Jeff explained what Model selection in the op was for adding cover\cap surfaces.

 

Mark

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


0 Likes

rumpelstielz
Collaborator
Collaborator

thanks so much for taking the time to help me out !


@Anonymous wrote:

So, normally when I open up someones file that they have shared, I generally figure out what they are trying to accomplish and find the one or 2 spots that they have had issues with.

Your file has presented a few more challenges than normal. When I first opened it up, it wasn't displaying the stock in Simulation mode. That puzzled me for a moment, until I realized that in your Setup, you didn't have any stock selected. It was set to "From Solid" but nothing was selected. Not sure if that was intentional, or something that got messed up in the export... That aside, let's start at T1, the 3mm endmill. You have collisions with that tool because the flutes are not long enough, on the 3rd drilling operation. Curious, why do you have 3 different drill operations using the same holes?


 

The lost model from the stock selection is something that happens to me from time to time when i open this file as well, not sure why this happens. I use the stock from solid a lot, not so much because i'm using non square stock but more so that i have a reference when positioning my model inside the stock. I also like to define my stocks through sketches so that if i have to machine a part again from a different stock dimension i can just adapt my stock model parameters quickly and can see it in the modeling workspace without having to go into the setup dialog in CAM.

 

As for the 3 drilling operations this is realted to the way i fix and prepare my stock (see also: http://forums.autodesk.com/t5/post-your-tips-and-tutorials/cam-the-toothpick-skewer-trick-or-the-poor-man-s-stock-fixture/m-p/6234870#M769 ). Here i was working of a piece of wood that was thicker than what i needed.

 

Drilling 1 (stockdrill high): put 4 fixing holes on the top of the thicker stock

Drilling 2 (bedDrill): put 4 fixing holes in my spoilboard

 

then i turn around the stock and fix it to the spoilboard with toothpicks. i then plane down the stock to the height i need (in this case 17mm). Since my stock is thicker than my mill is long i then drill another 4 holes in the back of the stock so i have identical fixture holes on each side which will be used for machining from both sides.

 


@Anonymous wrote:

Heights: Not a lot to say here, other than I notice that your WCS is way out in space and I wonder if that's intentional or.....? For bottom height you are saying "Model Bottom" plus another 3.9mm offset. Where does that put you on the part? Alternatively, you could also use Selection and select a face. It may be easier in the long run

 

Passes: Maximum Roughing Stepdown set to .5mm. Are you sure that's necessary? You posted a video the other day of how poor the simulation performance was. I see why now... .5mm stepdown is EXTREMELY light. More appropriate would be a rough step of .250" and a Fine Stepdown of .025"


 

my WCS is away from the world origin because this is part of a larger assembly (a guitar). By machining 'in place' it is easier for me to use the other parts of the model as a reference for modeling. Since i still switch around a lot between Rhino and Fusion this allows me to import/export parts and have them aligned on the model of the whole guitar.

 

The tiny roughing stepdown is due to the extremely weak spindle i have on my CNC. My machine is an old industrial engraving machine from the 1980's which i converted to a 3 axis Mach3 driven mill. The spindle motor has only 75W and to add insult to injury it's belt driven with a slip belt. In hardwoods (for this prototype i use mahogany) i can't really go any deeper than 0.5mm at a time, in Ebony (which will be the final part) i can only go 0.25mm at a time. Anything deeper than that would possibly stall my spindle.

I've been dying to change my spindle for one of those cheap chinese ones (100$ for a water cooled 1kw spindle), but unfortunately the way my machine is constructed i can't do this easily. I'd have to change the whole z-axis assembly which can't be easily done since it's not really a mill but an engraving machine and there is no easy way to just fix a spindle.

 

The weak spindle is also one of the resaons i use the adaptive strategy more like a pocket operation. As i understand it the adaptive strategy is meant to be used by cutting with the side of the mill whereas i tend to 'plunge machine' since my spindle can't handle such deep cuts.

 


@Anonymous wrote:

Geometry tab: You can leave it set to Silhouette if you want, or you can set it to Profile. Setting it to None will machine the entire part, stock included. Are you using bolts through the part to restrain it? If so, you don't want it set to None, as that will clear those out. Best bet would be to set it to Silhouette or Profile, Tool Outside Boundary as well as an Additional Offset of at least half the tool diameter.


 

yes i mostly use silhouete with tool outside boundary and an offset of a tiny bit more than half the tool diameter.


@Anonymous wrote:

Stock Contours. These really need to be turned on if you are trying to avoid crashing into stock. This is pretty much the main way you control how it "knows" where stock is. So, turn it on and select the profile of the stock you have modeled.

Model(s): Leave this field blank. The only thing it really is doing for you is increasing processing time. The Model is already selected in the Setup, so it's not going to cut through it by accident (assuming things are set proper). I know you are thinking that will control where the tool cuts, but that's not how it works. Hovering over the Model button gives you no info, and that's a shame. I think it's related to having multiple models in the setup, but I'm not certain. More info here would be nice. All I can say is that I never have to select anything at that point

 


 

i have to admit that even after your explanation and Marks screencast these two settings are the ones that most mystify me, especially since there doesn't seem to be any documentation or help on this, maybe someone from the Fusion team could explain exactly what the ideas behind these two settings are ? I usually select the model in the setup, when i run into problems like here i spend a lot of time trying to find solutions through trial and error, but the logic behind these two settings continues to elude me. What exactly is the purpose of being able to select models and stock contours here instead of their definition through the setup options ???


@Anonymous wrote:

Linking: And here is where a LOT of your collisions were coming from. You had the entry set to Plunge. That will drive the tool into the part at full rapid. You really should set it to Helix, if you are starting in the part. I'd also want to increase the Max Stay Down distance to a more realistic value, such as 1-2", that will reduce the amount of up/down that you would see


 

and this is the tab where i spent most time experimenting to get rid of the collissions, unfortunately without much success. I usually set the stay down distance pretty high but in this part it looked like that generated too much collisions so i set it really low to make sure there weren't any rapid travels to close to unmachined stock.


@Anonymous wrote:

So, in closing, I've attached your file with a few changes that I would be inclined to do.  Of course, I don't know the material you are working with, the rigity of your machine or even how you plan on holding this part.

 

I didn't go all out and look at every operation, just more the 3D adaptive. If you have ANY further questions, don't hesitate to ask

 


 i'll have a look at your file today and see if i can figure out more of the logic by comparing it with my experiments. Thanks so much for this, i still have a long way to go to fully understand Fusions machining but advice like this is super helpfull for my learning process.

 

BTW, here is the finished prototype part:

 

tailpiece_IMG_3475.jpg

 And here's the now almost finished guitar. The intital modeling and machining of body and neck was done in Rhino/Rhinocam, but the neck/pickup/control cavities where done in Fusion as well as the pickups, poti caps, tussrodcover and cavity covers. I'm currently preparing my next guitar which will hopefully be done entirely in Fusion.

 

01_front.jpg02_.jpg

==================================================
GENERAL DISCLAIMER: if there isn't a file attached to my posts then there is a reason for it. wherever i can i will attach a file for troubleshooting.If no file is attached i will always try to explain as clearly as possible with illustrative screenshots. when i have an issue that can only be helped by attaching a file which i cannot share publicly i won't ask about it here.
1 Like

rumpelstielz
Collaborator
Collaborator

@LibertyMachine: quick question, i'm looking at your file now but the units are in inches which makes it hard for me to compare to my settings since i work in metric. Is there a way to change the units for a design ? i searched for this but cannot seem to find a way to switch it.

==================================================
GENERAL DISCLAIMER: if there isn't a file attached to my posts then there is a reason for it. wherever i can i will attach a file for troubleshooting.If no file is attached i will always try to explain as clearly as possible with illustrative screenshots. when i have an issue that can only be helped by attaching a file which i cannot share publicly i won't ask about it here.
0 Likes

LibertyMachine
Mentor
Mentor

Yes, at the top of the tree on the left hand side (up above your Setup) is the units. Click on it and it will allow you to change it. Sorry, I'm a 'Merican and while I know how to use metric, it's more fluent for me to use Imperial


Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
0 Likes

LibertyMachine
Mentor
Mentor

@rumpelstielz wrote:

i have to admit that even after your explanation and Marks screencast these two settings are the ones that most mystify me, especially since there doesn't seem to be any documentation or help on this, maybe someone from the Fusion team could explain exactly what the ideas behind these two settings are ? I usually select the model in the setup, when i run into problems like here i spend a lot of time trying to find solutions through trial and error, but the logic behind these two settings continues to elude me. What exactly is the purpose of being able to select models and stock contours here instead of their definition through the setup options ???



 

Technically speaking, for Stock Contours, you often don't need to select anything, you just have to turn on the checkbox. Off; it makes no calculations against stock and will plunge into where there is material without a care. On; it will compare against what you have in the Setup. There is an exception to this: 2D Adaptive. Turning on Stock Contours will default to a rectangular stock size, regardless of what you have established in your Setup. You will need to select a profile if you use 3D adaptive.

 

In regards to the Model selection in the operations tab: I now understand it, thanks to @HughesTooling. It is there to assist you in applying proper toolpaths to parts that have features that would otherwise disrupt the tool flow. You can build a patch to cover cavities or cover over other features and include that into your toolpath, instead of selecting everything in the Setup model definition. In his video, you can see that the toolpath was going awry when it was encountering the engraving (extrusion into the part), He built a patch to cover over it and was able to select it when he applied the 3D contour to that face. With it selected, it was able to skip over the text without diving into it, like it (the text) wasn't there. My hack method (prior to grasping this concept) was to have 2 solid models, one with and one without certain features occupying the same spot. Turning the visibility on and off as needed was how I would get the results I wanted. Needless to say, I will not likely be suggesting that any further..


Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
0 Likes