Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Finish pass Facing Feed


Metallic
 Share

Recommended Posts

3 minutes ago, Leon82 said:

Hopefully one day this will be an option for facing and pockets.

I have been told you can use the tool path editor also

i was considering doing that, i havent really gotten into the details of toolpath editor. Any tutorial or resources you might have? I didnt even realize it was in there until recently

Link to comment
Share on other sites
1 minute ago, Metallic said:

i was considering doing that, i havent really gotten into the details of toolpath editor. Any tutorial or resources you might have? I didnt even realize it was in there until recently

I've never used it personally. I have been meaning to find the time but never do

Link to comment
Share on other sites
1 hour ago, Metallic said:

Maybe i am being blind, but how can I modify the feed rate for a finishing pass on a facing toolpath? I figure there has to be an easier way that copy/pasting?

 

Thanks in advance

What I typically do is setup 2 separate operations to handle the roughing and finishing.

In the first Operation, I disable Clearance and Retract, but first I change the options for both to "0.0" and "Incremental". I set the Feed Plane to 0.0 Incremental.

I set the depth (typically), to how ever much stock I want to leave (say .040), and set it to Incremental.

If I am doing several depth cuts, I set the Top of Stock to the correct value as Incremental from my depth. (Say .500 for example.)

Then I set my Max Depth value. In this case we are starting at .500 above Z Zero with the stock, and leaving. 040, so we are removing 0.460 of stock. I'll set my max depth step value to .100. That means we take the total depth (.46), divided by the Max Step value (.100), and we get  4.6 as the answer.

Mastercam uses the max depth as a limit. So when a division is made, and the number is not a whole number, the system round the value up to the nearest whole integer, and performs the calculation again. (0.46 ÷ 5 = .092 per pass)

So Mastercam would rough each step as 5 depth cuts of .092 thick per pass. Or if we can push the tool deeper than .100, we simply divide the total depth by the actual number of passes we want. For example, 0.46 ÷ 4 = .115 per pass. So we set our max step to .115 and we get 4 depth passes.

Now, in the Reference Points, we add an "Approach" point of Incremental (Z only) set to 2. Or 4. Inches. This gives us our initial approach point to start the cutting.

Because we have the depths set to .04 Incremental and the Clearance and Retract disabled, the tool will not retract at the end of the Operation.

We can then copy and paste the Operation. Disable Depth Cuts, set Depth to 0. (Same for TOS and Feed Plane). Adjust speeds and feeds.

Now, disable the Approach Point, and add a Retract Point, for Z Incremental, at whatever hight you want.

So, the first Operation uses Approach Point to get the Tool to the start. Then the Op roughs the material, leaving some on the floor for Finish. Important: the tool does not retract in the NCI Data. The 2nd Op has "no approach move", so the tool simply moves to the start point between Ops. The 2nd Op cuts the floor with finish parameters. (Often I will kick up the stepover from 65% for roughing, to 90% for finishing), and adjusted  speed feed values. The 2nd Op uses a Retraction Reference Point to get the tool raised back up to a safe location.

 

  • Thanks 1
  • Like 3
Link to comment
Share on other sites
9 hours ago, Colin Gilchrist said:

What I typically do is setup 2 separate operations to handle the roughing and finishing.

In the first Operation, I disable Clearance and Retract, but first I change the options for both to "0.0" and "Incremental". I set the Feed Plane to 0.0 Incremental.

I set the depth (typically), to how ever much stock I want to leave (say .040), and set it to Incremental.

If I am doing several depth cuts, I set the Top of Stock to the correct value as Incremental from my depth. (Say .500 for example.)

Then I set my Max Depth value. In this case we are starting at .500 above Z Zero with the stock, and leaving. 040, so we are removing 0.460 of stock. I'll set my max depth step value to .100. That means we take the total depth (.46), divided by the Max Step value (.100), and we get  4.6 as the answer.

Mastercam uses the max depth as a limit. So when a division is made, and the number is not a whole number, the system round the value up to the nearest whole integer, and performs the calculation again. (0.46 ÷ 5 = .092 per pass)

So Mastercam would rough each step as 5 depth cuts of .092 thick per pass. Or if we can push the tool deeper than .100, we simply divide the total depth by the actual number of passes we want. For example, 0.46 ÷ 4 = .115 per pass. So we set our max step to .115 and we get 4 depth passes.

Now, in the Reference Points, we add an "Approach" point of Incremental (Z only) set to 2. Or 4. Inches. This gives us our initial approach point to start the cutting.

Because we have the depths set to .04 Incremental and the Clearance and Retract disabled, the tool will not retract at the end of the Operation.

We can then copy and paste the Operation. Disable Depth Cuts, set Depth to 0. (Same for TOS and Feed Plane). Adjust speeds and feeds.

Now, disable the Approach Point, and add a Retract Point, for Z Incremental, at whatever hight you want.

So, the first Operation uses Approach Point to get the Tool to the start. Then the Op roughs the material, leaving some on the floor for Finish. Important: the tool does not retract in the NCI Data. The 2nd Op has "no approach move", so the tool simply moves to the start point between Ops. The 2nd Op cuts the floor with finish parameters. (Often I will kick up the stepover from 65% for roughing, to 90% for finishing), and adjusted  speed feed values. The 2nd Op uses a Retraction Reference Point to get the tool raised back up to a safe location.

 

That's a handy trick and I use it for ops other than facing.  Especially in 5 axis where don't want to force tc but keep the tool down for null tool changes.

 

I wish I knew as much as Colin has forgotten.

  • Like 1
Link to comment
Share on other sites
14 hours ago, Colin Gilchrist said:

So, the first Operation uses Approach Point to get the Tool to the start. Then the Op roughs the material, leaving some on the floor for Finish. Important: the tool does not retract in the NCI Data. The 2nd Op has "no approach move", so the tool simply moves to the start point between Ops. The 2nd Op cuts the floor with finish parameters. (Often I will kick up the stepover from 65% for roughing, to 90% for finishing), and adjusted  speed feed values. The 2nd Op uses a Retraction Reference Point to get the tool raised back up to a safe location.

 

This makes sense for sure, I just wish there was a simpler way built into the toolpath. Oh well.

 

Thanks for the detailed explanation to make it easier

Link to comment
Share on other sites
On 11/27/2018 at 4:19 PM, jlw™ said:

This is a good suggestion, you can use the pocket path for facing:

Capture.png

and then use the finishing tab:

Capture2.png

Use zigzag and under cut parameters, set wall to -(half of cutter + lead in/out).

I’d never even thought of using Pocket to face a top surface with no features. I’ll try this tomorrow thanks 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...