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

4th axis vice toolpath help

CHAY.HOBSON
Enthusiast

4th axis vice toolpath help

CHAY.HOBSON
Enthusiast
Enthusiast

When I export this code to the HAAS it runs the tool path for the angled edges in mid air. I feel like I've tried every option in Tool Orientation but it just does the same thing! Is it something to do with the set up?

CHAYHOBSON_0-1649251381211.png

 

0 Likes
Reply
Accepted solutions (1)
730 Views
16 Replies
Replies (16)

engineguy
Mentor
Mentor

@CHAY.HOBSON 

 

Yes, it is likely your Setup, try changing it to the position shown in the image below, everything should then rotate around that point and should work :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

Simple stem front.jpg

 

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast

Thanks. I tried that and still the same result. The 4th axis vice indexes then the toolpath runs to the side of the part. It seems to be more of an issue with the Y - Axis. I've tried the et up in the centre of vice rotation and that doesn't work either. I've tried with 2d parallel and 3d face toolpaths and still the same result. 

0 Likes

engineguy
Mentor
Mentor

@CHAY.HOBSON 

 

OK, few things to look at, the part/stock must be physically set up the same in Fusion and the machine. If the center of the part/stock that is aligned with the rotating center of the 4th axis as in my image then that is how it needs to be fixed in the machine.

Are you using the HAAS DWO and TCP ?

Which Post Processor ar you using Pre NGC or NGC

Which Axis is the 4th axis mounted along on the Machine ? X axis or Y axis ?

 

Can you upload a copy of the Post Processor that you are using ?

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast

Yes, the WCS is replicated with the G54 in the machine. I’m using the HAAS VF-1 with the HRT160 (5th axis vice fitted) 4th axis running along the X-axis. Post processing using HAAS pre NGC 4th axis. I’m back at home now so don’t have access to the code but it’s on the file I put on the original post. 

0 Likes

engineguy
Mentor
Mentor

@CHAY.HOBSON 

 

Try the attached file, run the simulation first and then generate the code, it should work as long as the piece of stock is setup exactly as the stock in the Fusion file, with the bottom center line aligned with the center of the 4th axis.

Simple stem front.jpg

 

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast

@engineguy I have tried this but can try again. The centre of the stock Z not the bottom is in the centre of the vice. The only file I can see that's attached is the photo....

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast

This is the actual centre of rotation. Should the set up be mill or mill turn? 

 

CHAYHOBSON_0-1649316958769.png

 

0 Likes

engineguy
Mentor
Mentor

@CHAY.HOBSON 

 

Apologies, forgot to attach the file, here it is again, now it is set to the middle of the Stock as in your image, if that is how it is actually fixed in the machine then this attempt should be a lot closer :slightly_smiling_face:

 

Setup should be set to "Milling".

Simple stem front.jpg

 

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast

This has worked!! Thank you for all your help. What had I done wrong? 

0 Likes

engineguy
Mentor
Mentor

@CHAY.HOBSON 

 

Glad you have it working.

 

Really all that was wrong was getting the center of rotation in the correct place, it is just a matter of how the Stock is fixed to the 4th axis compared to what is set in Fusion, they have to match :slightly_smiling_face:

 

Originally you had the rotation point set to the top of your stock and then I did one with it set to the bottom but you did have the stock set in the 4th axis to the center of the stock so selecting that point made it work :slightly_smiling_face:

 

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast
I've put my flow toolpath back in and it's doing the same thing again so it must be something to do with that! The flow tool path was the only way I could get the internal wrap. I had tried it first with the the WCS at the centre of rotation.
0 Likes

engineguy
Mentor
Mentor

@CHAY.HOBSON 

 

You don`t need the Flow to machine out that area, in fact for what you are doing you don`t need the Machining Extension at all, you are just doing 3+1 machining.

I used the Blend as the finishing Toolpath and it works fine, if you want it to go from side to side in the same direction as the Flow then change the "Drive Curve" selection from the two side edges to the two end arcs, what you will get then is just movement in the Z and Y axes, it should do the job OK.

 

I am not able to check any of your Flow settings as I don`t have that Extension which is why I tend to use the 3D options available :slightly_smiling_face: :slightly_smiling_face: :slightly_smiling_face:

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast

It looks like it doesn't quite get right to the corners with angle restraint but I will give it a try. 

 

CHAYHOBSON_0-1649332193891.png

 

0 Likes

engineguy
Mentor
Mentor

@CHAY.HOBSON 

 

Why would you need a restraint ??

Runs on the center of the tool right to the edge ??

0 Likes

CHAY.HOBSON
Enthusiast
Enthusiast

@engineguy OK, so I've figured it out! I ran your toolpaths again straight out of the model you sent and this time it machined mid air! For some reason my post processor auto checks this box "rotate A-axis the opposite direction" When I uncheck this box all the toolpaths work!!

CHAYHOBSON_0-1649336037162.png

If you look at the difference in these 2 toolpaths it looks as if the tool on the blend doesn't get to the the top edges but it is just using the side of the tool.

CHAYHOBSON_1-1649336301644.png

 

The Flow toolpath maintains machining using the end of the tool. 

 

CHAYHOBSON_2-1649336371075.png

Thank you so much for all your help! It is very much appreciated. 

 

 

0 Likes

engineguy
Mentor
Mentor
Accepted solution

@CHAY.HOBSON 

 

By using the Blend you get the tool using the curve of the Radius instead of just the Tip of the tool all the time, usually results in a smoother finish.

The Blend does it by default but if you are using for example the Parallel for the finish then you can set the toolpath to use the Tip or not option, see image below for how it works :slightly_smiling_face:

Simple Stem Contact.jpg

 

Simple Stem Contact-1.jpg

 

Hope that helps :slightly_smiling_face:

1 Like